SINUMERIK. SINUMERIK 840D sl / 828D Measuring cycles. Preface. Fundamental safety instructions 1. Description 2. Measuring variants 3

Transcription

1 Preface Fundamental safety instructions 1 SINUMERIK SINUMERIK 840D sl / 828D Description 2 Measuring variants 3 Parameter lists 4 Programming Manual Changes from cycle version SW4.4 and higher Appendix A B Valid for: Control system SINUMERIK 840D sl / 840DE sl / 828D Software CNC software version 4.7 SP2 SINUMERIK Operate for PCU/PC version 4.7 SP2 10/2015 6FC5398-4BP40-5BA3

2 Legal information Warning notice system This manual contains notices you have to observe in order to ensure your personal safety, as well as to prevent damage to property. The notices referring to your personal safety are highlighted in the manual by a safety alert symbol, notices referring only to property damage have no safety alert symbol. These notices shown below are graded according to the degree of danger. DANGER indicates that death or severe personal injury will result if proper precautions are not taken. WARNING indicates that death or severe personal injury may result if proper precautions are not taken. CAUTION indicates that minor personal injury can result if proper precautions are not taken. NOTICE indicates that property damage can result if proper precautions are not taken. If more than one degree of danger is present, the warning notice representing the highest degree of danger will be used. A notice warning of injury to persons with a safety alert symbol may also include a warning relating to property damage. Qualified Personnel The product/system described in this documentation may be operated only by personnel qualified for the specific task in accordance with the relevant documentation, in particular its warning notices and safety instructions. Qualified personnel are those who, based on their training and experience, are capable of identifying risks and avoiding potential hazards when working with these products/systems. Proper use of Siemens products Note the following: Trademarks WARNING Siemens products may only be used for the applications described in the catalog and in the relevant technical documentation. If products and components from other manufacturers are used, these must be recommended or approved by Siemens. Proper transport, storage, installation, assembly, commissioning, operation and maintenance are required to ensure that the products operate safely and without any problems. The permissible ambient conditions must be complied with. The information in the relevant documentation must be observed. All names identified by are registered trademarks of Siemens AG. The remaining trademarks in this publication may be trademarks whose use by third parties for their own purposes could violate the rights of the owner. Disclaimer of Liability We have reviewed the contents of this publication to ensure consistency with the hardware and software described. Since variance cannot be precluded entirely, we cannot guarantee full consistency. However, the information in this publication is reviewed regularly and any necessary corrections are included in subsequent editions. Siemens AG Division Digital Factory Postfach NÜRNBERG GERMANY Document order number: 6FC5398-4BP40-5BA3 P 01/2016 Subject to change Copyright Siemens AG All rights reserved

3 Preface SINUMERIK documentation The SINUMERIK documentation is organized in the following categories: General documentation User documentation Manufacturer/service documentation Additional information You can find information on the following topics at Ordering documentation/overview of documentation Additional links to download documents Using documentation online (find and search in manuals/information) Please send any questions about the technical documentation (e.g. suggestions for improvement, corrections) to the following address: My Documentation Manager (MDM) Under the following link you will find information to individually compile OEM-specific machine documentation based on the Siemens content: Training For information about the range of training courses, refer under: SITRAIN - Siemens training for products, systems and solutions in automation technology SinuTrain - training software for SINUMERIK FAQs You can find Frequently Asked Questions in the Service&Support pages under Product Support. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 5

4 Preface SINUMERIK You can find information on SINUMERIK under the following link: Target group This programming manual is intended for machine tool programmers for the SINUMERIK Operate software. Benefits With the programming manual, the target group can develop, write, test, and debug programs and software user interfaces. Standard scope This documentation only describes the functionality of the standard version. Additions or revisions made by the machine manufacturer are documented by the machine manufacturer. Other functions not described in this documentation might be executable in the control. This does not, however, represent an obligation to supply such functions with a new control or when servicing. For the sake of simplicity, this documentation does not contain all detailed information about all types of the product and cannot cover every conceivable case of installation, operation, or maintenance. Technical Support You will find telephone numbers for other countries for technical support in the Internet under 6 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

5 Table of contents Preface Fundamental safety instructions General safety instructions Industrial security Description Basics General prerequisites Behavior on block search, dry run, program testing, simulation Reference points on the machine and workpiece Definition of the planes, tool types Probes that can be used Probe, calibration body, calibration tool Measuring workpieces on milling machines, machining centers Measuring tools on milling machines, machining centers Measuring workpieces at the turning machines Measuring tools at lathes Measurement principle Measuring strategy for measuring workpieces with tool offset Parameters for checking the measurement result and offset Effect of empirical value, mean value, and tolerance parameters Measuring cycle help programs CYCLE116: Calculation of center point and radius of a circle CYCLE119: Arithmetic cycle for determining position in space CUST_MEACYC: User program before/after measurements are performed Miscellaneous functions Measuring cycle support in the program editor Measuring result screens Logging General Control cycle CYCLE Log "Last measurement" Standard log User log Behavior during block search, simulation and for several channels Measuring variants General requirements Overview of the measuring cycles...71 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 7

6 Table of contents Selection of the measuring variants via softkeys (turning) Selection of the measuring variants via softkeys (milling) Result parameters Measure workpiece (turning) General information Calibrate probe - length (CYCLE973) Calibrate probe - radius on surface (CYCLE973) Calibrate probe - calibrate in groove (CYCLE973) Turning measurement - front edge (CYCLE974) Turning measurement - inside diameter (CYCLE974, CYCLE994) Turning measurement - outside diameter (CYCLE974, CYCLE994) Extended measurement Measure workpiece (milling) General information Calibrate probe - length (CYCLE976) Function Calling the measuring version Parameters Result parameters Calibrate probe - radius in ring (CYCLE976) Calibrate probe - radius on edge (CYCLE976) Calibrate probe - radius between 2 edges (Cycle976) Function Calling the measuring version Result parameters Calibrate probe - calibrate on ball (CYCLE976) Edge distance - set edge (CYCLE978) Edge distance - align edge (CYCLE998) Edge distance - groove (CYCLE977) Edge distance - rib (CYCLE977) Corner - right-angled corner (CYCLE961) Corner - any corner (CYCLE961) Hole - rectangular pocket (CYCLE977) Hole - 1 hole (CYCLE977) Hole - inner circle segment (CYCLE979) Spigot - rectangular spigot (CYCLE977) Spigot - 1 circular spigot (CYCLE977) Spigot - outer circle segment (CYCLE979) D - align plane (CYCLE998) D - sphere (CYCLE997) D - 3 spheres (CYCLE997) D - angular deviation spindle (CYCLE995) D - kinematics (CYCLE996) Expanded functionality CYCLE Checking the sphere diameter Scaling of rotary axis vectors V1 and V D measuring on machines with orientation transformation Measuring the workpiece on a machine with combined technologies Measuring a workpiece on a milling/turning machine Measuring a workpiece on a turning/milling machine Allocating the trigger values Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

7 Table of contents Uniformity when using a 3D probe of type Measure tool (turning) General information Calibrate probe (CYCLE982) Turning tool (CYCLE982) Milling tool (CYCLE982) Drill (CYCLE982) Measure tool with toolholder that can be orientated Measure tool (milling) General information Calibrate probe (CYCLE971) Milling tool (CYCLE971) Measurement with stationary spindle Measurement with rotating spindle Cutting tooth breakage monitoring Calling the measuring version Parameters Result parameters Measuring the tool on machines with combined technologies Drill (CYCLE971) Calling the measuring version Parameters Result parameters Parameter lists A 4.1 Overview of measuring cycle parameters CYCLE973 measuring cycle parameters CYCLE974 measuring cycle parameters CYCLE994 measuring cycle parameters CYCLE976 measuring cycle parameters CYCLE978 measuring cycle parameters CYCLE998 measuring cycle parameters CYCLE977 measuring cycle parameters CYCLE961 measuring cycle parameters CYCLE979 measuring cycle parameters CYCLE997 measuring cycle parameters CYCLE995 measuring cycle parameters CYCLE996 measuring cycle parameters CYCLE982 measuring cycle parameters CYCLE971 measuring cycle parameters CYCLE150 measuring cycle parameters Additional parameters Additional result parameters Parameter Changes from cycle version SW4.4 and higher A.1 Assignment of the measuring cycle parameters to MEA_FUNCTION_MASK parameters A.2 Changes in the machine and setting data from SW A.3 Complete overview of the changed cycle machine and cycle setting data Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 9

8 Table of contents B A.4 Comparing GUD parameters (regarding measuring functions) A.5 Changes to names of cycle programs and GUD modules Appendix B.1 Abbreviations B.2 Documentation overview Glossary Index Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

9 Fundamental safety instructions General safety instructions WARNING Risk of death if the safety instructions and remaining risks are not carefully observed If the safety instructions and residual risks are not observed in the associated hardware documentation, accidents involving severe injuries or death can occur. Observe the safety instructions given in the hardware documentation. Consider the residual risks for the risk evaluation. WARNING Danger to life or malfunctions of the machine as a result of incorrect or changed parameterization As a result of incorrect or changed parameterization, machines can malfunction, which in turn can lead to injuries or death. Protect the parameterization (parameter assignments) against unauthorized access. Respond to possible malfunctions by applying suitable measures (e.g. EMERGENCY STOP or EMERGENCY OFF). Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 11

10 Fundamental safety instructions 1.2 Industrial security 1.2 Industrial security Note Industrial security Siemens provides products and solutions with industrial security functions that support the secure operation of plants, solutions, machines, equipment and/or networks. They are important components in a holistic industrial security concept. With this in mind, Siemens products and solutions undergo continuous development. Siemens recommends strongly that you regularly check for product updates. For the secure operation of Siemens products and solutions, it is necessary to take suitable preventive action (e.g. cell protection concept) and integrate each component into a holistic, state-of-the-art industrial security concept. Third-party products that may be in use should also be considered. For more information about industrial security, visit this address ( To stay informed about product updates as they occur, sign up for a product-specific newsletter. For more information, visit this address ( WARNING Danger as a result of unsafe operating states resulting from software manipulation Software manipulation (e.g. by viruses, Trojan horses, malware, worms) can cause unsafe operating states to develop in your installation which can result in death, severe injuries and/ or material damage. Keep the software up to date. You will find relevant information and newsletters at this address ( support.automation.siemens.com). Incorporate the automation and drive components into a holistic, state-of-the-art industrial security concept for the installation or machine. You will find further information at this address ( industrialsecurity). Make sure that you include all installed products into the holistic industrial security concept. 12 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

11 Description Basics General information are general subroutines designed to solve specific measurement tasks. They can be adapted to specific problems via parameter settings. When taking general measurements, a distinction is made between Tool measurement and Workpiece measurement. Workpiece measurement Workpiece measurement, turning example Workpiece measurement, milling example In workpiece measurement, a probe is moved up to the clamped workpiece in the same way as a tool and the measured values are acquired. The flexibility of measuring cycles makes it possible to perform nearly all measurements required on a milling or turning machine. The result of the workpiece measurement can be optionally used as follows: Compensation in the work offset Automatic tool offset Measurement without offset Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 13

12 Description 2.1 Basics Tool measurement Tool measurement, turning tool example Tool measurement, drill example In tool measurement, the selected tool is moved up to the probe and the measured values are acquired. The probe is either in a fixed position or is swung into the working area with a mechanism. The tool geometry measured is entered in the appropriate tool offset data set. 14 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

13 Description 2.2 General prerequisites 2.2 General prerequisites Certain preconditions must be met before measuring cycles can be used. These are described in detail in the SINUMERIK 840D sl Base Software and Operating Software. Check the preconditions using the following checklist: Machine All machine axes are designed in accordance with DIN Machine data has been adapted. Starting position The reference points have been approached. The starting position can be reached by linear interpolation without collision. Display functions of the measuring cycles A HMI/PCU or HMI/TCU is required for showing the measuring result displays and for measuring cycle support. Please observe the following when programming: Tool radius compensation is deselected before it is called (G40). The cycle is called no later than at the 5th program level. The measurement is also possible in a system of units that differs from the basic system (with technology data that has been switched over). For metric dimension system with active G70, G700. For inch dimension system with active G71, G710. References Supplementary information for this documentation is provided in the following manuals: Commissioning Manual SINUMERIK 840D sl Base Software and Operating Software /IM9/ SINUMERIK Operate /PG/, Programming Manual SINUMERIK 840D sl / 828D Fundamentals /FB1/, Function Manual Basic Functions /FB2/, Function Manual Expanded Functions /FB3/, Function Manual Special Functions Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 15

14 Description 2.3 Behavior on block search, dry run, program testing, simulation 2.3 Behavior on block search, dry run, program testing, simulation Function The measuring cycles are skipped during execution if one of the following execution modes is active: "Trial run" ($P_DRYRUN=1) "Program test" ($P_ISTEST=1) "Block search" ($P_SEARCH=1), only if $A_PROTO=0. Simulation and simultaneous recording Setting the measuring cycles under a simulated environment Setting data SD55618 $SCS_MEA_SIM_ENABLE = 0: The measuring cycles are exited without any function. = 1: The measuring cycles are executed. -Simulation in the HMI Operate editor: Traversing motion is visualized. No measurement results and measurement result display are available. -SinuTrain: = 2 to 8: Reserved For simultaneous recording, measurement results and measurement result display are available. For simultaneous recording traversing motion is visualized. -For systems that exclusively work with simulated axes (e.g. virtual machines, test racks): For simultaneous recording, measurement results and measurement result display are available. For simultaneous recording traversing motion is visualized. The following settings should be noted: if MD13230 $MN_MEAS_PROBE_SOURCE = 1 to 4, then set MD10360 $MN_FASTIO_DIG_NUM_OUTPUTS >= 1. = 9: Internal or for special applications, if MD13230 >=1 and measurement results under a simulated environment (SinuTrain) are used for programming for training purposes if a real machine is not available. The measurement results also involve "simulated" values, which can also deviate from the setting in MD13213 MEAS_PROBE_OFFSET. 16 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

15 Description 2.3 Behavior on block search, dry run, program testing, simulation Image 2-1 Measuring - simulation Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 17

16 Description 2.4 Reference points on the machine and workpiece 2.4 Reference points on the machine and workpiece General information Depending on the measuring task, measured values may be required in the machine coordinate system (MCS) or in the workpiece coordinate system (WCS). For example: It may be easier to ascertain the tool length in the machine coordinate system. Workpiece dimensions are measured in the workpiece coordinate system. Where: M = machine zero in the machine coordinate system W = workpiece zero in the workpiece coordinate system F = tool reference point Reference points The position of tool reference point F in the machine coordinate system is defined with machine zero M as the machine actual value. The position of the tip/cutting edge of the active tool in the workpiece coordinate system is displayed with the workpiece zero W as workpiece actual value. For a workpiece probe, the center or the end of the probe ball can be defined as the tool tip. The work offset (WO) characterizes the position of the workpiece zero W in the machine coordinate system. Work offsets (WO) comprise the components offset, rotation, mirroring and scaling factor (only the global basis work offset does not contain any rotation). A distinction is made between the basis, work offset (G54... G599) and programmable work offset. The basic area contains further subsections such as the basic work offset, channelspecific basic work offset and configuration-dependent work offsets (e.g. rotary table reference or basic reference). 18 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

17 Description 2.4 Reference points on the machine and workpiece The specified work offsets are effective together as a chain and result in the workpiece coordinate system. For "Correction in a work offset", in conjunction with measuring cycles, a distinction is made between two different cases. Correction to the coarse offset: An absolute offset value is determined between the machine zero and the measured workpieces zero. This offset is written into the coarse component of the selected work offset and deleted in the fine component. Correction to the fine offset: The measured difference is written as offset to the fine component of the selected work offset and is added to the course component. The input window work offset coarse/fine in the automatic measuring cycle screens is activated using SD54760 $SNS_MEA_FUNCTION_MASK_PIECE, bit 10 = 1. Note Scale factors with a scaling value unequal to "1" are not supported by the measuring cycles! Mirroring functions are only permitted in conjunction with counterspindles on lathes. The machine and workpiece coordinate system can be set and programmed separately in the "inch" or "metric" measuring system. Note Transformation Measure workpiece Workpiece measurements are always performed in the workpiece coordinate system. All descriptions relating to workpiece measurement refer to it! Measure tool When measuring tools with kinematic transformation active, a distinction is made between basic coordinate system and machine coordinate system. If kinematic transformation is deactivated, this distinction is made. All subsequent descriptions relating to tool measurement assume that kinematic transformation is disabled and therefore refer to the machine coordinate system. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 19

18 Description 2.5 Definition of the planes, tool types 2.5 Definition of the planes, tool types When measuring under milling, machining planes G17, G18 or G19 can be selected. When measuring under turning, machining plane G18 must be selected. For tool measurement, the following tool types are permitted: Milling, type 1.. Drill, type 2... Turning tools, type 5... Depending on the tool type, the tool lengths are assigned to the axes as follows: Workpiece probe, milling: Probe types 710, 712, 713, 714 Workpiece probe, turning: Probe type 580 for turning machines without extended milling technology, otherwise 710 See "Measuring the workpiece on a machine with combined technologies (Page 229)". Milling Acts in... G17 plane G18 plane G19 plane Tool type: 1xy / 2xy / 710 Length 1 1st axis of the plane: Z Y X Length 2 2nd axis of the plane: Y X Z Length 3 3rd axis of the plane: X Z Y Note: In the assignment of the tool lengths, note the settings in the following setting data SD42940 $SC_TOOL_LENGTH_CONST SD42950 $SC_TOOL_LENGTH_TYPE 20 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

19 Description 2.5 Definition of the planes, tool types Example of plane definition for milling Image 2-2 Example: Milling machine with G17 Turning Turning machines generally only use axes Z and X and therefore: G18 plane Tool type Length 1 Length 2 5xy (turning tool, workpiece probe) Acts in X (2nd axis of the plane) Acts in Z (1st axis of the plane) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 21

20 Description 2.5 Definition of the planes, tool types G17 and G19 are used for milling on a turning machine. If there is no machine axis Y, milling can be implemented with the following kinematic transformations. TRANSMIT TRACYL In principle, measuring cycles support kinematic transformations. This is stated more clearly in the individual cycles and measuring variants. Information about kinematic transformation can be found in the Programming Manual SINUMERIK 840D sl / 828D Fundamentals or in the documentation of the machine manufacturer. Note If a drill or milling cutter is measured on a lathe, in most cases, the channel-specific SD $SC_TOOL_LENGTH_TYPE = 2 is set: These tools are then length-compensated like a turning tool. SINUMERIK controls have other machine and setting data that can influence the calculation of a tool. References: /FB1/, Function Manual Basic Functions /FB2/, Function Manual Expanded Functions /FB3/, Function Manual Special Functions Example of plane definition for turning Image 2-3 Example: Lathe with G18 22 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

21 Description 2.6 Probes that can be used 2.6 Probes that can be used General information To measure tool and workpiece dimensions, an electronic touch-trigger probe is required that provides a signal change (edge) when deflected with the required repeat accuracy. The probe must operate virtually bounce-free. Different types of probe are offered by different manufacturers. Note Please observe the information provided by the manufacturers of electronic probes and/or the machine manufacturer's instructions on the following points: Electrical connection Mechanical calibration of the probe If a workpiece probe is used, both the direction of deflection and transmission of switching signal to the machine column (radio, infrared or cable) must be taken into account. In some versions, transmission is only possible in particular spindle positions or in particular ranges. This can restrict the use of the probe. Probes are distinguished according to the number of measuring directions. Multi-directional (multi probe) Mono-directional (mono probe) Workpiece probe Tool probe Multi-directional (3D) Mono-directional Milling machines Lathes The probes also differ in the form of the stylus tip: The measuring cycles support pin, L and star probes as autonomous tool types. The use of the probe types is referenced in the individual measuring cycles. The multi probe is universally applicable. For a mono probe, the switching direction is tracked for each measurement by turning the spindle. This can lead to a longer program runtime. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 23

22 Description 2.6 Probes that can be used Workpiece probe types The following workpiece measuring probe types as well as a calibration tool for calibrating tool probes are provided in the tool management: Image 2-4 Probe types in the tool management Tool data from probes The probes differ as a result of the tool type and their special attributes, e.g. switching directions. A probe can encompass several tool types. For this purpose, several cutting edges (D1, D2,...) should be created for the probe. Example: Multi probe with a boom D1 3D_PROBE Type 710 D2 L_PROBE Type 713 The user must take into account the geometry of the probe when pre-positioning. To do this, you can read out individual tool data in the user program: Example: IF (($P_TOOLNO>0) AND ($P_TOOL>0)) ENDIF R1= ($P_AD[6]) ; Reading: tool radius of the current tool Correction angle "The probe is aligned in the +X direction using tool parameter "correction angle". 24 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

23 Description 2.6 Probes that can be used 3D probe (multi probe) Display Properties Characteristic Application: Universal Type: $TC_DP1 = 710 Tool length: in Z (for G17) 1) Correction angle: $TC_DP10 = 0.0 to Radius of the probe sphere $TC_DP6 1) Workpiece measurement, length reference of the 3D probe The tool length in the direction of the infeed axis (for G17: Z axis) is defined as the distance between the tool reference point in the tool adapter and a parameterized reference point on the probe sphere. The reference point can be set to the center of the sphere or the surface of the sphere using the following machine data: MD51740 $MN_MEA_FUNCTION_MASK, bit 1 Mono probe Display Properties Characteristic Application: Type: $TC_DP1 = 712 Tool length: in Z (for G17) 1) Alignment of the switching direction when measuring Correction angle: $TC_DP10 = 0.0 to Radius of the probe sphere $TC_DP6 1) Workpiece measurement, length reference of mono probe The tool length in the direction of the infeed axis (for G17: Z axis) is defined as the distance between the tool reference point in the tool adapter and a parameterized reference point on the probe sphere. The reference point can be set to the center of the sphere or the surface of the sphere using the following machine data: MD51740 $MN_MEA_FUNCTION_MASK, bit 1 As initial state for the measuring cycles it is defined that at spindle position 0 the switching direction of the mono probe in the machining plane is aligned in the axis direction +X. If an angular offset is required, then the value should be entered into tool parameter "Correction angle" ($TC_DP10). Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 25

24 Description 2.6 Probes that can be used L probe Display Properties Characteristic Application: Towing measurement in +Z Type: $TC_DP1 = 713 Tool length: in Z (for G17) 1) Correction angle: $TC_DP10 = 0.0 to Radius of the probe sphere: Length of the boom: 1) Workpiece measurement, length reference $TC_DP6 $TC_DP7 The tool length is defined as the distance between the tool reference point in the tool adapter and the probing point of the probe sphere in the +Z direction. As initial state for the measuring cycles it is defined that at spindle position 0 the switching direction of the mono probe in the machining plane is aligned in the axis direction +X. If an angular offset is required, then the value should be entered into tool parameter "Correction angle" ($TC_DP10). Star probe Display Properties Characteristic Application: Measure: Hole parallel to the axis 1) Type: $TC_DP1 = 714 Tool length: in Z (for G17) 2) Correction angle: $TC_DP10 = 0.0 to Diameter of the star parallel to the geometry axes: Radius of the probe sphere: $TC_DP6 $TC_DP7 1) The application only refers to measurements in the plane (for G17: XY plane). Measurement in the tool direction (for G17: Z direction) is not permitted using a star probe. If a measurement is to be made in the tool direction, a star element (boom) must be parameterized as an L probe ($TC_DP1 = 713). 2) Workpiece measurement, length reference of star probe The tool length is defined as the distance between the tool reference point in the tool adapter and the center point of one of the probe spheres. The booms of the star probe should be aligned parallel to the geometry axes of the machining plane. If an angular offset is required, then the value should be entered into tool parameter "Correction angle" ($TC_DP10). Assignment of the probe types Probe type Lathes Milling and machining centers Tool measurement Workpiece measurement Workpiece measurement Multi-directional X X X Mono-directional X 26 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

25 Description 2.7 Probe, calibration body, calibration tool 2.7 Probe, calibration body, calibration tool Measuring workpieces on milling machines, machining centers Probe calibration All probes must be mechanically correctly adjusted before use. The switching directions must be calibrated before they are used in the measuring cycles for first-time. This also applies when changing the stylus tip of the probe. When being calibrated, the trigger points (switching points), position deviation (skew), and active sphere radius of the workpiece probe are determined and entered into the data fields of the general setting data SD $SNS_MEA_WP_BALL_DIAM. There are 12 data fields. Calibration can be realized in a calibration ring (known bore), on a calibration sphere or on workpiece surfaces, which have an appropriate geometrical precision and low surface roughness. Use the same measuring velocity for calibrating and measuring. This applies in particular to the feedrate overide. If, in MD51740 $MNS_MEA_FUNCTION_MASK, bit 6 is set =1, then 100% feed rate override traversing velocity is used for the measuring blocks (MEAS) in the measuring cycles if the feedrate override is set > 0. If calibration is performed more than once on a calibration data set, the same measuring velocity must be set, otherwise the previous calibration will be declared as being invalid. Measuring cycle CYCLE976 with different measuring versions is available to calibrate the probe. Measuring All probe types can be used in conjunction with a spindle capable of positioning. This ensures that all milling measuring versions can be applied. When positioning the probe, the measuring cycles always refer to the active master spindle. If several spindles exist, then this condition must be satisfied by the user. During the program runtime, this is possible using the SETMS NC command. Example: SETMS(3); the third spindle is defined as master spindle. If probes are used in conjunction with spindles that are not capable of positioning, restrictions are obtained regarding the measuring versions and probe types. For illegal measuring versions, alarms can be displayed during the cycle time. At the calibration and measurement instant, the user must guarantee an identical orientation (spindle position) of the probe, for example by clamping or indexing. If probes are fixed in a system, restrictions are obtained regarding the measuring versions and probe types. For illegal measuring versions, alarms can be displayed during the cycle time. When the probe is mounted in the machine at a fixed position, a mechanical offset can exist in the three geometry axes between the center point of the probe sphere (tool tip) and the tool reference point. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 27

26 Description 2.7 Probe, calibration body, calibration tool This offset should be entered in the adapter dimension (basis dimension) of the tool data of the workpiece probe. See also Calibrate probe - radius in ring (CYCLE976) (Page 111) Calibrate probe - radius on edge (CYCLE976) (Page 116) Calibrate probe - calibrate on ball (CYCLE976) (Page 122) Measuring tools on milling machines, machining centers Tool probe Image 2-5 Measuring a milling cutter 28 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

27 Description 2.7 Probe, calibration body, calibration tool Parameters of the tool probe Setting data For machine-related measurement/calibration: SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX1 SD $SNS_MEA_TP_TRIG_PLUS_DIR_AX1 SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX2 SD $SNS_MEA_TP_TRIG_PLUS_DIR_AX2 SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX3 SD $SNS_MEA_TP_TRIG_PLUS_DIR_AX3 For machine-related measurement/calibration: SD $SNS_MEA_TPW_TRIG_MINUS_DIR_AX1 SD $SNS_MEA_TPW_TRIG_PLUS_DIR_AX1 SD $SNS_MEA_TPW_TRIG_MINUS_DIR_AX2 SD $SNS_MEA_TPW_TRIG_PLUS_DIR_AX2 SD $SNS_MEA_TPW_TRIG_MINUS_DIR_AX3 SD $SNS_MEA_TPW_TRIG_PLUS_DIR_AX3 The default setting has data fields for 6 probes. Calibration, calibration tool A probe must be calibrated before it can be used. To do this, when using measuring cycles in the AUTOMATIC mode, before calibration, the approximate values must be entered into the setting data listed above for the corresponding probe. Only then can the approximate position of the probe be identified in the measuring cycle. Calibration involves precisely determining the trigger points (switching points) of the tool probe, and entering them in the corresponding parameters. Calibration tool (type 725), milling (type 1xy) or drilling tool (2xy) can be used for calibration. The precise dimensions of the tool are known. Measurement version Calibrate probe (CYCLE971) (Page 259) is provided for calibration. Note Measuring velocities It is recommended that the same measuring velocities are used for calibrating and measuring. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 29

28 Description 2.7 Probe, calibration body, calibration tool Tool parameters Calibrating tool probes Tool type ($TC_DP1[ ]): Length 1 - geometry ($TC_DP3[ ]): Radius ($TC_DP6[ ]): Length 1 - basic dimension ($TC_DP21[ ]): 725, 1xy or 2xy L1 r only if required All other tool parameters, such as wear, must be assigned a value of zero Measuring workpieces at the turning machines Workpiece probe On turning machines, the workpiece probes are treated as tool type 5xy with permissible cutting edge positions (SL) 5 to 8 and must be entered in the tool memory accordingly. Lengths specified for turning tools always refer to the tool tip, except in the case of workpiece probes on turning machines where they refer to the probe center. Probes are classified according to their position: Workpiece probe SL 7 Entry in tool memory Workpiece probe for a lathe Tool type ($TC_DP1[ ]): Cutting edge ($TC_DP2[ ]): 7 Length 1 - geometry: Length 2 - geometry: Radius ($TC_DP6[ ]): Length 1 - basic dimension ($TC_DP21[ ]): Length 2 - basic dimension ($TC_DP22[ ]): 5xy L1 L2 r only if required only if required The wear and other tool parameters must be assigned the value Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

29 Description 2.7 Probe, calibration body, calibration tool Workpiece probe SL 8 Entry in tool memory Workpiece probe for a lathe Tool type ($TC_DP1[ ]): Cutting edge ($TC_DP2[ ]): 8 Length 1 - geometry: Length 2 - geometry: Radius ($TC_DP6[ ]): Length 1 - basic dimension ($TC_DP21[ ]): Length 2 - basic dimension ($TC_DP22[ ]): 5xy L1 L2 r only if required only if required The wear and other tool parameters must be assigned the value 0. Workpiece probe SL 5 or SL 6 Entry in tool memory Workpiece probe for a lathe Tool type ($TC_DP1[ ]): 5xy Cutting edge ($TC_DP2[ ]): 5 or 6 Length 1 - geometry: Length 2 - geometry: Radius ($TC_DP6[ ]): Length 1 - basic dimension ($TC_DP21[ ]): Length 2 - basic dimension ($TC_DP22[ ]): L1 L2 r only if required only if required The wear and other tool parameters must be assigned the value 0. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 31

30 Description 2.7 Probe, calibration body, calibration tool Calibration, gauging block Image 2-6 Calibrating a workpiece probe, example: Calibrating in the reference groove A probe must be calibrated before it can be used. When being calibrated, the trigger points (switching points), position deviation (skew), and precise ball radius of the workpiece probe are determined and entered into the corresponding data fields of the general setting data SD $SNS_MEA_WP_BALL_DIAM. The default setting has data fields for 12 probes. Calibration of the workpiece probe on turning machines is usually performed with gauging blocks (reference grooves). The precise dimensions of the reference groove are known and entered in the associated data fields of the following general setting data: SD54615 $SNS_MEA_CAL_EDGE_BASE_AX1 SD54616 $SNS_MEA_CAL_EDGE_UPPER_AX1 SD54617 $SNS_MEA_CAL_EDGE_PLUS_DIR_AX1 SD54618 $SNS_MEA_CAL_EDGE_MINUS_DIR_AX1 SD54619 $SNS_MEA_CAL_EDGE_BASE_AX2 SD54620 $SNS_MEA_CAL_EDGE_UPPER_AX2 SD54621 $SNS_MEA_CAL_EDGE_PLUS_DIR_AX2 SD54622 $SNS_MEA_CAL_EDGE_MINUS_DIR_AX2 The default setting has data fields for three gauging blocks. In the measuring cycle program, the selection is made using the number of the gauging block (S_CALNUM). It is also possible to calibrate on a known surface. Measuring cycle CYCLE973 with various measuring versions is ready for calibration. 32 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

31 Description 2.7 Probe, calibration body, calibration tool See also Calibrate probe - length (CYCLE973) (Page 80) Calibrate probe - radius on surface (CYCLE973) (Page 82) Calibrate probe - calibrate in groove (CYCLE973) (Page 85) Measuring tools at lathes Tool probe Image 2-7 Measuring a turning tool Parameters of the tool probe Setting data: For machine-related measurement/calibration: SD $SNS_MEA_TP_TRIG_PLUS_DIR_AX1 SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX1 SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX2 SD $SNS_MEA_TP_TRIG_PLUS_DIR_AX2 For workpiece-related measurement/calibration: SD $SNS_MEA_TPW_TRIG_PLUS_DIR_AX1 SD $SNS_MEA_TPW_TRIG_MINUS_DIR_AX1 SD $SNS_MEA_TPW_TRIG_MINUS_DIR_AX2 SD $SNS_MEA_TPW_TRIG_PLUS_DIR_AX2 The default setting has data fields for 6 probes. In addition to turning tools, drills and mills can also be measured. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 33

32 Description 2.7 Probe, calibration body, calibration tool Calibration, gauging block A probe must be calibrated before it can be used. To do this, when using measuring cycles in the AUTOMATIC mode, before calibration, the approximate values must be entered into the setting data listed above for the corresponding probe. Only then can the approximate position of the probe be identified in the measuring cycle. Calibration involves precisely determining the trigger points (switching points) of the tool probe, and entering them in the corresponding parameters. Calibration tool (type 585 or type 725) or turning tool (type 5xy) can be used for calibration. The precise dimensions of the tool are known. Measurement version Calibrate probe (CYCLE982) (Page 234) is provided for calibration. For lathes, the calibration tool is treated like a turning tool. Cutting edge positions 1-4 can be used for calibration. The lengths refer to the sphere equator, not to the sphere center. Entry in tool memory Tool type ($TC_DP1[ ]): Cutting edge ($TC_DP2[ ]): 3 Length 1 - geometry: Length 2 - geometry: Radius ($TC_DP6[ ]): Length 1 - basic dimension ($TC_DP21[ ]): Length 2 - basic dimension ($TC_DP22[ ]): 585, 725 or 5xy L1 L2 r only if required only if required Calibration tool for a tool probe on a lathe All other parameters, such as wear, must be assigned a value of zero. 34 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

33 Description 2.8 Measurement principle 2.8 Measurement principle Flying measurement The principle of "flying measurement" is implemented in the SINUMERIK control. The probe signal is processed directly on the NC so that the delay when acquiring measured values is minimal. This permits a higher measuring speed for the prescribed measuring precision and time needed for measuring is reduced. Connecting probes Two inputs for connecting touch trigger probes are provided on the I/O device interface of the SINUMERIK control systems. Machine manufacturer Please observe the machine manufacturer s instructions. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 35

34 Description 2.8 Measurement principle Measurement operation sequence using the example set edge (CYCLE978) Image 2-8 Measurement operation sequence, example set edge (CYCLE978) The sequence is described using the measuring version, set edge (CYCLE978). The sequence is essentially the same for the other measuring cycles. The starting position for the measuring procedure is the position DFA in front of the specified set position (expected contour). Image 2-9 Starting position The starting position is calculated in the cycle based on parameter entries and probe data. The traversing distance from the pre-position, defined by the user program, to the starting position of the measuring distance is either traversed with rapid traverse G0 or with positioning speed G1 (depending on the parameter). From the starting position, the measuring velocity is effective, which is saved in the calibration data. The switching signal is expected along path 2 DFA as from the starting position. Otherwise, an alarm will be triggered or the measurement repeated. 36 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

35 Description 2.8 Measurement principle The resulting maximum measuring position is available in the result parameters _OVR[ ] and _OVI[ ] of the measuring cycle. At the instant the switching signal is output by the probe, the current actual position is stored internally "on-the-fly" as the actual value, the measuring axis is stopped and then the "Delete distance-to-go" function is executed. The distance-to-go is the path not yet covered in the measuring block. After deletion, the next block in the cycle can be processed. The measuring axis travels back to the starting position. Any measurement repetitions selected are restarted from this point. Measurement path DFA Measurement path DFA defines the distance between the starting position and the expected switching position (setpoint) of the probe. Measuring velocity As measuring feedrate, all of the measuring cycles use the value saved in the general setting data SD54611 after the calibration of the workpiece probe. A different measuring feedrate can be assigned for each calibration field [n]. To calibrate the measuring probe, either the measuring feedrate from the channel-specific setting data SD55630 $SCS_MEA_FEED_MEASURE is used (default value: 300 mm/min) or the measuring feedrate can be overridden in the input screen form at the calibration instant. To do this, bit 4 must be set to 1 in the general setting data SD54760 $SNS_MEA_FUNCTION_MASK_PIECE. The maximum permissible measuring velocity is derived from: The deceleration behavior of the axis. The permissible deflection of the probe. The signal processing delay. Deceleration distance, deflection of probe NOTICE Safe braking of the measuring axis Safe deceleration of the measuring axis to standstill within the permissible deflection path of the probe must always be ensured. Otherwise damage will occur! A delay t, typical for the control, is taken into account in signal processing (IPO cycle) for the time between detection of the switching signal and output of the deceleration command to the measuring axis: general machine data MD10050 $MN_SYSCLOCK_CYCLE_TIME and MD10070 $MN_IPO_SYSCLOCK_TIME_RATIO). This gives the braking distance component. The following error of the measuring axis is reduced. The following error is velocity dependent and at the same time dependent on the control factor of the measuring axis (servo gain of the associated machine axis: servo gain factor). Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 37

36 Description 2.8 Measurement principle The deceleration rate of the axis must also be taken into account. Together they produce an axis-specific velocity-dependent deceleration distance. The Kv factor is the axis MD $MA_POSCTRL_GAIN. The maximum axis acceleration / deceleration rate a is saved in axis MD $MA_MAX_AX_ACCEL. It may have a lesser effect due to other influences. Always use the lowest values of the axes involved in the measurement. Measuring accuracy A delay occurs between detection of the switching signal from the probe and transfer of the measured value to the control. This is caused by signal transmission from the probe and is defined by the control hardware. In this time a path is traversed that falsifies the measured value. This influence can be minimized by reducing the measuring speed. The rotation when measuring a milling tool on a rotating spindle has an additional influence. This can be compensated using compensation tables. The measurement accuracy that can be obtained is dependent on the following factors: Repeat accuracy of the machine Repeat accuracy of the probe Resolution of the measuring system Note Precise measurement is only possible with a probe calibrated under the measurement conditions, i.e. working plane, orientation of the spindle in the plane and measuring velocity are the same for both measurement and calibration. Deviations result in measurement errors. If, in MD51740 $MNS_MEA_FUNCTION_MASK, bit 6 is set =1, then 100% feed rate override traversing velocity is used for the measuring blocks (MEAS) in the measuring cycles if the feedrate override is set > Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

37 Description 2.8 Measurement principle Calculating the deceleration distance Image 2-10 Distance-time diagram at different measuring velocities according to the calculation example The deceleration path to be considered is calculated as follows: s b Braking distance in mm v Measuring velocity in m/s t Delay signal in s a Deceleration in m/s 2 Δs Following error in mm Δs = v / Kv v here in m/min Kv Servo gain in (m/min)/mm Example of calculation: v = 6 m/min = 0.1 m/s measuring velocity a = 1 m/s 2 deceleration t = 16 ms signal delay Kv = 1 in (m/min)/mm Intermediate steps: Δs = v / Kv = 6[m/min] / 1[(m/min)/mm] = 6 mm Following error Δs 2 = v²/2a = 0,1 [m/s]² / 2 1 [m/s²] = 5 mm Axis-specific component Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 39

38 Description 2.8 Measurement principle Δs 1 = v t = 0,1 [m/s] 0,016 [s] = 1,6 mm Percentage due to signal delay Overall result: s b = Δs 1 + Δs 2 + Δs = 6 mm + 5 mm + 1,6 mm = 12,6 mm Braking distance The deflection of the probe = braking distance to zero speed of the axis is 12.6 mm. 40 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

39 Description 2.9 Measuring strategy for measuring workpieces with tool offset 2.9 Measuring strategy for measuring workpieces with tool offset The actual workpiece dimensions must be measured exactly and compared with the setpoint values to be able to determine and compensate the actual dimensional deviations on the workpiece. An offset value can then be ascertained for the tool used for machining. Function When taking measurements on the machine, the actual dimensions are derived from the path measuring systems of the position-controlled feed axes. For each dimensional deviation determined from the set and actual workpiece dimensions there are many causes which essentially fall into three categories: Dimensional deviations with causes that are n o t subject to a particular trend, e.g. positioning scatter of the feed axes or differences in measurement between the internal measurement (probe) and the external measuring device (micrometer, measuring machine, etc.). In this case, it is possible to apply empirical values, which are stored in separate memories. The set/actual difference determined is automatically compensated by the empirical value. Dimensional deviations with causes that a r e subject to a particular trend, e.g. tool wear or thermal expansion of the leadscrew. Accidental dimensional deviations, e.g. due to temperature fluctuations, coolant or slightly soiled measuring points. Assuming the ideal case, only those dimensional deviations that are subject to a trend can be taken into account for compensation value calculation. Since, however, it is hardly ever known to what extent and in which direction accidental dimensional deviations influence the measurement result, a strategy (sliding averaging) is needed that derives a compensation value from the actual/set difference measured. Mean value calculation Mean value calculation in conjunction with measurement weighting has proven a suitable method. When correcting a tool, it can be selected whether a correction is made based on the actual measurement, or whether an average value of the measurement differences should be generated over several measurements which is then used to make the correction. The formula of the mean value generation chosen is: Mv new = Mv old - Mv old k - D i Mv new Mv old k D i Mean value new = amount of compensation Mean value prior to last measurement Weighting factor for mean value calculation Actual/set difference measured (minus any empirical value) The mean value calculation takes account of the trend of the dimensional deviations of a machining series. The weighting factor k from which the mean value is derived is selectable. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 41

40 Description 2.9 Measuring strategy for measuring workpieces with tool offset A new measurement result affected by accidental dimensional deviations only influences the new tool offset to some extent, depending on the weighting factor. Computational characteristic of the mean value with different weightings k Image 2-11 Mean value generation with influence of weighting k The greater the value of k, the slower the formula will respond when major deviations occur in computation or counter compensation. At the same time, however, accidental scatter will be reduced as k increases. The lower the value of k, the faster the formula will react when major deviations occur in computation or counter compensation. However, the effect of accidental variations will be that much greater. The mean value Mv is calculated starting at 0 over the number of workpieces i, until the calculated mean value exceeds the work offset range (S_TZL). From this limit on, the calculated mean value is applied as an offset. Once the mean value has been used for the offset, it is deleted from the memory. The next measurement then starts again with Mv old = Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

41 Description 2.9 Measuring strategy for measuring workpieces with tool offset Table 2-1 Example of mean value calculation and offset 1. measurement 2. Measurement 3. Measurement 4. Measurement 5. Measurement 6. Measurement 7. Measurement 8. Measurement 9. Measurement 10. Measurement i Lower limit = 40 µm (S_TZL = 0.04) Di [µm] Mv k = 3 [µm] Mv k = 2 [µm] ,3 32, ,5 46, , , ,4 37, ,3 1 43, , , Characteristic of the mean value for two different weighting factors For the measurements with marked fields, tool offset is performed with the mean value (calculated mean value >S_TZL): If k=3 in the 7th and 10th measurement (1 and 2), If k=2 in the 3rd, 7th, and 9th measurement (3, 4 and 5). Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 43

42 Description 2.10 Parameters for checking the measurement result and offset 2.10 Parameters for checking the measurement result and offset For constant deviations not subject to a trend, the dimensional deviation measured can be compensated by an empirical value in certain measuring variants. For other compensations resulting from dimensional deviations, symmetrical tolerance bands are assigned to the set dimension which result in different responses. Empirical value / mean value EVN (S_EVNUM) The empirical values are used to suppress dimensional deviations that are not subject to a trend. Note If empirical values are not to be applied, then S_EVNUM = 0 must be set. The empirical values themselves are saved in channel-specific SD $SCS_MEA_EMPIRIC_VALUE. EVN specifies the number of the empirical value memory. The actual/set difference determined by the measuring cycle is corrected by this value before any further correction measures are taken. This is the case: For workpiece measurement with automatic tool offset. For single-point measurement with automatic WO correction. For tool measurement. The mean value only refers to the workpiece measurement with automatic tool offset. For an automatic tool offset, the mean value is generated from the measured difference of the previous and the actual measurement. This functionality has special significance within a machining series with measurements performed at the same measuring location. The function does not have to be activated. The mean values are stored in the channel-specific SD $SCS_MEA_AVERAGE_VALUE.The number of the mean value memory is transferred in the measuring cycle using variable S_EVNUM. Safe area TSA (S_TSA) The safe area is effective for almost all measuring variants and does not affect the offset value; it is used for diagnostics. 44 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

43 Description 2.10 Parameters for checking the measurement result and offset If this limit is reached then the following can be assumed: A probe defect, or An incorrect setpoint position, or An illegal deviation from the setpoint position can be assumed. Note AUTOMATIC mode AUTOMATIC operation is interrupted and the program cannot continue. An alarm text appears to warn the user. Dimension difference check DIF (S_TDIF) DIF is active only for workpiece measurement with automatic tool offset and for tool measurement. This limit has no effect on generation of the compensation value either. When it is reached, the tool is probably worn and needs to be replaced. Note An alarm text is displayed to warn the operator and the program can be continued by means of an NC start. This tolerance limit is generally used by the PLC for tool management purposes (twin tools, wear monitoring). Tolerance of workpiece: Lower limit (S_TLL), upper limit (S_TUL) Both parameters are active only for tool measurement with automatic tool offset. When measuring a dimensional deviation ranging between "2/3 tolerance of workpiece" (S_TMV) and "Dimensional difference control" (S_TDIF), this is regarded 100% as tool offset. The previous average value is erased. This enables a fast response to major dimensional deviations. Note When the tolerance limit of the workpiece is exceeded, this is indicated to the user depending on the tolerance position "oversize" or "undersize". 2/3 tolerance of workpiece TMV (S_TMV) TMV is active only for workpiece measurement with automatic tool offset. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 45

44 Description 2.10 Parameters for checking the measurement result and offset Within the range of "Lower limit" and "2/3 workpiece tolerance" the mean value is calculated according to the formula described in Section "Measuring strategy". Note Mv new is compared with the work offset range: If Mv new is greater than this range, compensation is corrected by Mv new and the associated mean value memory is cleared. If Mv new is less than this range, no compensation is carried out. This prevents excessively abrupt compensations. Weighting factor for mean value generation FW (S_K) FW is active only for workpiece measurement with automatic tool offset. The weighting factor can be used to give a different weighting for each measurement. A new measurement result thus has only a limited effect on the new tool offset as a function of FW. Work offset range TZL (S_TZL) TZL active for Workpiece measurement with automatic tool offset Tool measurement and calibration for milling tools and tool probes This tolerance range corresponds to the amount of maximum accidental dimensional deviations. It has to be determined for each machine. No tool compensation is made within these limits. In workpiece measurement with automatic tool offset, however, the mean value of this measuring point is updated and re-stored with the measured actual/set difference, possibly compensated by an empirical value. 46 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

45 Description 2.10 Parameters for checking the measurement result and offset The tolerance bands (range of permissible dimensional tolerance) and the responses derived from them are as follows: For workpiece measurement with automatic tool offset Note In measuring cycles, the workpiece setpoint dimension is placed in the middle of the permitted ± tolerance limit for reasons associated with symmetry. For tool measurement Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 47

46 Description 2.10 Parameters for checking the measurement result and offset For workpiece measurement with WO correction For workpiece probe calibration For tool probe calibration 48 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

47 Description 2.11 Effect of empirical value, mean value, and tolerance parameters 2.11 Effect of empirical value, mean value, and tolerance parameters The following flowchart shows the effect of empirical value, mean value, and tolerance parameters on workpiece measurement with automatic tool offset. 1 SD $SNS_MEA_FUNCTION_MASK, Bit 0 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 49

48 Description 2.11 Effect of empirical value, mean value, and tolerance parameters 50 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

49 Description 2.12 Measuring cycle help programs 2.12 Measuring cycle help programs CYCLE116: Calculation of center point and radius of a circle Function This cycle calculates from three or four points positioned on one plane the circle they inscribe with center point and radius. To allow this cycle to be used as universally as possible, its data is transferred via a parameter list. An array of REAL variables of length 13 must be transferred as the parameter. Image 2-12 Calculation of circle data from 4 points Programming CYCLE116 (_CAL[ ], _MODE) Transfer parameters Input data Parameters Data type Meaning _CAL [0] REAL Number of points for calculation (3 or 4) _CAL [1] REAL 1. Axis of the plane of the first point _CAL [2] REAL 2. Axis of the plane of the first point _CAL [3] REAL 1. Axis of the plane of the second point _CAL [4] REAL 2. Axis of the plane of the second point _CAL [5] REAL 1. Axis of the plane of the third point _CAL [6] REAL 2. Axis of the plane of the third point Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 51

50 Description 2.12 Measuring cycle help programs Parameters Data type Meaning _CAL [7] REAL 1. Axis of the plane of the fourth point _CAL [8] REAL 2. Axis of the plane of the fourth point Output data Parameters Data type Meaning _CAL [9] REAL 1. Axis of the plane of the circle center point _CAL [10] REAL 2. Axis of the plane of the circle center point _CAL [11] REAL Circle radius _CAL [12] REAL Status for the calculation 0 = Calculation in progress 1 = Error occurred _MODE INTEGER Error number (61316 or possible) Note This cycle is called as a subroutine by, for example, measuring cycle CYCLE979. Example %_N_Circle_MPF DEF INT _MODE DEF REAL _CAL[13]= (3,0,10,-10,0,0,-10,0,0,0,0,0,0) ;3 points specified P1: 0,10 P2: -10,0 P3: 0,-10 CYCLE116(_CAL[ ], _MODE) ;Result: _CAL[9]=0 _CAL[10]=0 _CAL[11]=10 _CAL[12]=0 _ALM=0 M0 STOPRE M30 52 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

51 Description 2.12 Measuring cycle help programs CYCLE119: Arithmetic cycle for determining position in space Function This help cycle calculates, from three spatial setpoint positions (reference triangle), three spatial actual positions as well as the positional and angular deviation to the active frame. The offset is applied in the direction of the selected frame. Cycle119 is separately called from measuring cycle CYCLE997 as subprogram or from a user program. To universally use this cycle, its data are transferred via a parameter interface. Programming CYCLE119 (_SETPOINT, _MEASPOINT, _ALARM, _RES, _REFRAME,_COR, _RESLIM) Parameter Input data Data type Meaning _SETPOINT[3, 3] _MEASPOINT[3,3] REAL REAL _COR INTEGER Compensation Field for 3 setpoint positions in the sequence 1st, 2nd, 3rd, geometry axis (X, Y, Z). These points are the reference triangle. Field for 3 setpoint positions measured in the sequence 1st, 2nd, 3rd, geometry axis (X, Y, Z). This is really the spatial position of the defined triangle. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 53

52 Description 2.12 Measuring cycle help programs Input data Data type Meaning Values: 0: No compensation : WO compensation in G54...G57, G505..G : WO compensation in last active channel basic frame according to MD to 1026: WO compensation in channel basic frame 2000: WO compensation in system frame for scratching and setting actual value ($P_SETFR). 9999: WO compensation in active frame, settable frame G54 to G57, G505...G599 and/or with G500 in last active basic frame according to $P_CHBFRMASK _RESLIM REAL Limit value for distortion (only relevant, if _COR >0 ). If _RES is below this value, then WO is compensated, otherwise an alarm is output. Output data Data type Meaning The results of the calculation are stored in these transfer parameters. _ALARM INTEGER Cycle alarm number for feedback signal. _RES REAL Calculation result (for cycle call, transfer value must be = 0.) Values: < 0: No frame was able to be calculated. Alarm (_ALARM > 0) is returned >= 0: The calculation was successful. The size of the value a measure of the distortion of the triangle, for example, due to measurement inaccuracies. It is the sum of the deviations of the individual points in mm. _REFRAME FRAME Result frame, difference to the active frame. If this result frame is linked with the active frame, the measured triangle position is given the desired setpoint position (workpiece coordinates). Note For correction The frame to be corrected must not include any mirroring or scale factors. If there is no channel basic frame for G500, then a cyclic alarm (_ALARM>0) is output. If cycle 119 is called by cycle 997, then the corrected frame is automatically activated. If cycle 119 is separately called in a user program, the new data of the frame are activated outside the cycle when the G command of the associated adjustable frame (G500, G54 up to...) is reprogrammed CUST_MEACYC: User program before/after measurements are performed Function The CUST_MEACYC cycle is called in every measuring cycle before and after the measurement. 54 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

53 Description 2.12 Measuring cycle help programs It can be used by users to program sequences necessary before starting a measurement (e.g. to activate the probe). In the as-delivered state, this cycle contains a CASE statement that executes a jump to a label with subsequent M17 (end of subprogram) for each measuring cycle. Example _M977: GOTOF _AM_WP_MES ;... ; _AM_WP_M ES: ; ; M17 ;before workpiece probe with CYCLE977(measure hole/shaft/groove/spigot) ;before workpiece general ;end of cycle From the jump labels, actions can be programmed, which should be executed at each CYCLE977 call (label _M977) all for general workpiece measurements (label _AM_WP_MES). References Commissioning manual SINUMERIK 840D sl Basesoftware and Operating Software. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 55

54 Description 2.13 Miscellaneous functions 2.13 Miscellaneous functions Measuring cycle support in the program editor The program editor offers extended measuring cycle support for inserting measuring cycle calls into the program. Prerequisite Hardware TCU or PCU. Function This measuring cycle support provides the following functionality: Measuring cycle selection via softkeys Input screen forms for parameter assignment with help displays Retranslatable program code is generated from the individual screen forms Measuring result screens Function Measurement result displays can be shown automatically during a measuring cycle. The measurement result screen display can now be called in the program using cycle CYCLE150, which also controls the logging function. Measuring result screens Procedure The part program or ShopMill program to be processed has been created and is opened in the editor. 1. Press the "Meas. workpiece" or "Meas. tool" softkey. 2. Press the "Meas. result" softkey. The "Measurement result" input window opens. 3. Make the required selection in the toggle fields. The display mode can be selected as follows in the screen for the measurement result display "on": 56 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

55 Description 2.13 Miscellaneous functions - "automatically 8 s"... The measurement result screen remains for a fixed time of 8 s - "NC Start"... With the measurement result screen, the cycle is stopped using M0, the measuring cycle is continued with NC Start and the measurement result screen deselected - "for alarm"... The measuring results screen is only displayed for cycle alarms 61303, 61304, and These selection options correspond to the options that were previously available using SD55613 $SCS_MEA_RESULT_DISPLAY. Measurement result screen display and logging function can be separately activated and deactivated. An additional CYCLE150 call should be programmed. At the end of the program (channel RESET), the function is deactivated automatically, explicit programming is not required. Note For compatibility reasons, the previous option of controlling the measurement result screen display using setting data $SCS_MEA_RESULT_DISPLAY has been kept. The measuring cycles can display different measuring result screens depending on the measuring variant: Calibrating tool probes Tool measurement Calibrating workpiece probes Workpiece measurement Content of measuring result screens The measuring results screens contain the following data: Calibrating the tool probe Measuring cycle and measuring version Trigger values of axis directions and differences Probe number Safe area Tool measurement Measuring cycle and measuring version Actual values and differences for tool offsets Safe area and permissible dimensional difference T name, D number Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 57

56 Description 2.13 Miscellaneous functions Calibrating workpiece probes Measuring cycle and measuring version Trigger values of axis directions and differences Position deviation (probe skew) when calibrating in the plane Probe number Safe area Workpiece measurement Measuring cycle and measuring version Setpoints, actual values and their differences Tolerance upper and lower limits (for tool offset) Offset value Probe number Safe area and permissible dimensional difference T name, D number and DL number or WO memory number for automatic offset Example of measurement result display 58 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

57 Description 2.13 Miscellaneous functions Program control for displaying and shutting down the measuring result displays Using the program control MRD "Display measurement result", programmed measuring result display calls can be simply activated or deactivated. To do this, the program does not have to be changed! The program control MRD acts on all measuring result display calls, irrespective of whether they are implemented using CYCLE150 calls or by programming setting data $SCS_MEA_RESULT_DISPLAY in the program Logging General Function Standard log Output of the measurement results from the automatic measuring cycles in a log file. Each measuring method of the standard measuring cycles is assigned a fixed standard log with regard to the contents. The contents correspond to the measurement result display on the screen. User entries for the log contents are not required. User log Output of user-relevant data as a separate log or supplement to the measurement log. The contents and format are the sole responsibility of the user. A predefined variable field is available which can take the contents of the log. It is possible to log to external media, if they are available, on local drives, USB or in the part program memory. The log output can be in text format or in tabular format (column separator ";") for further processing in spreadsheet programs. Requirements If the data is to be logged to external media or network drives, then the EES mode must be set (see "Commissioning Manual Sinumerik Operate (IM9)"). Contents of a standard log Date/time (when the log was written), log name with path Measuring method The most important input values (that were entered in the screen form before measuring) Correction target Setpoints, measured values and differences As many decimal places are logged as displayed on the screen. The terms and axis names also correspond to those displayed on the screen but are written out (without abbreviations). The measurement unit mm/inch depends on the system of units active during the measurement. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 59

58 Description 2.13 Miscellaneous functions Control cycle CYCLE150 Function The activation of the logging function is performed by simply programming the CYCLE150 call. The result display and logging can be selected separately and can be controlled independently. Parameters in CYCLE150 have a modal effect until the end of the program or reset, or until the cycle is called again. Procedure The logging is activated and deactivated via the program through the appropriate parameterization of CYCLE150. This must be programmed once at the start of the measuring program. Only when the input parameters are changed must the programming be performed again before the respective measuring cycle call. At the end of the program (channel RESET), the functions are deactivated automatically, explicit programming is not required. The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" or "Meas. tool" softkey. 2. Press the "Meas. result" softkey. The "Measurement Result" input window opens. 3. Make the required selection in the toggle fields (see following table). The screen form contains a selection field for activating and deactivating the measurement result display with the toggle states "Off"/"On". It also contains a selection field for activating and deactivating the logging with the toggle states "Off"/"On"/"Last measurement". If both selections fields have the toggle state "Off", all the following input fields for the respective function are hidden. Parameter Parameter Measurement result display Display mode Log Log type Log format (for standard) Log data Log storage Name of log file Description Off/On autom. 8 s / NC start / for alarm Standard log / User log Text format / Tabular format (file extension TXT/CSV) New/Append Directory / As part program File type set according to selection of log format 60 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

59 Description 2.13 Miscellaneous functions Log type The existing infrastructure for the logging of the measurement results should also be made accessible to users for their own purposes - output of user logs. A distinction is therefore made between the standard log and the user log. Log format Standard logs can be output in two log formats, in text format and in tabular format. The text format is based on the display of the measurement results on the screen. The tabular format is a format that can be imported by Excel (or other spreadsheet programs). This allows the measurement result logs to be statistically processed. The Text format / Tabular format selection is only available for standard logs. With user logs, the user is responsible for the formatting, i.e. the selection field is hidden for the user log. Log data A new log file can be created or an existing file appended. This is selected via Log data "New" or "Append". With "New", the existing file with the same name is deleted and a new file created during logging. Log storage The path can be specified explicitly or implicitly for the log storage, i.e. "Directory" or "As part program" can be selected. With "As part program", the path of the higher-level NC program is automatically determined by the logging cycles and the log file is stored there. The following input field for the path is hidden. With "Directory", there is an additional input field in which the path is entered. The path does not have to be entered, it can be selected via a dialog which is opened via the additional VSK1 "Select directory". Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 61

60 Description 2.13 Miscellaneous functions Image 2-13 Entry level in the selection dialog for log storage This softkey "Select directory" only appears when "Directory" is set in the Log storage selection field. Image 2-14 Selection dialog for log storage All drives and paths available in the program manager can be selected. Local drive NC data (part program memory) Network drive(s), if connected USB (if available) Only a path or an available file can be selected in the dialog. If only a path is selected, the selection with the complete path is transferred to the screen form with the Accept softkey, but can be changed. The name of the log file is entered. If a file is selected, the full path and file name are transferred to the screen form, but can be changed. Alternatively, the storage location can be entered. 62 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

61 Description 2.13 Miscellaneous functions Examples of the selected storage location: 1. NC data -> Workpiece -> Workpiece "Logs" //NC/WCS.DIR/LOGS.WPD 2. Network drive logs //d:/logs 3. USB -> measuring_cycle_logs //USB:/01/measuring_cycle_logs Name of log file The log file name can be freely selected. It must comply with the rules for program names in the NC, or for program names when writing to external drives. File type The following file types are supported: Text file - type TXT Tabular format type CSV These file types depend on the selected log format. The file type cannot be changed, it is only displayed Log "Last measurement" Function The "Log last measurement" function is programmed by calling the logging CYCLE150 once. Measuring is not performed, instead the values of the last measurement which are still available in the result parameters of the measuring cycles (GUD variables) are used, and only a subcycle is called for the logging. This function only makes sense when log "Off" was selected during the measurement. Requirement A standard log can only be output when a measuring cycle was previously active in automatic mode. Procedure A part program for logging "Last measurement" is created and is in the editor. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 63

62 Description 2.13 Miscellaneous functions 1. Select Log "Last measurement" in the input field. 2. Supply additional parameters as described above. 3. Press the "Accept" softkey. The generated cycle call appears in the editor. Programming example: CYCLE150(30,11012,"//NC/MPF.DIR/LAST_MEASURE.TXT") M Standard log Function Standard logs display the results from measuring cycles in a clear log structure. The output is possible in text or tabular format. Contents and structure are predefined. Requirement Standard logs are only possible in conjunction with measuring cycle calls. Log contents The logs are generally created with fixed English texts. (The measurement result displays appear in the language that has been set for Operate.) Logs of the measuring cycles have the following structures and contents: Header block - log header Date/time (when the log was created) Name and path of the log file Name of the part program from which the measuring function was called Workpiece number Value block - results per measuring point Number of the measuring point, measuring method as programmed, time of the measurement Measuring method as text (e.g. "1 hole") Specification of the correction target, either measure only no correction or for measuring methods with WO correction: Specification of the corrected WO, correction target (WO / fine offset) or For measuring methods with tool offset: Tool name, D number, tool type, correction target (length/radius, geometry/wear) Setpoints, measured values, differences with specification of the respective axis name or measurement objects (e.g. "Diameter") and the measurement unit 64 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

63 Description 2.13 Miscellaneous functions Procedure The call of the control CYCLE150 is always at the start of the program. The respective measuring cycle calls are then programmed. If a different parameterization of CYCLE150 is required, it must be called again at the appropriate program position. Programming example N10 G54 N20 T710 D1 M6 ; Probe call... ; Positioning, etc. N50 CYCLE150(10,1001,"MESSPROT.TXT") ; Activate logging N60 ; 1st measurement CYCLE997(109,1,1,10,1,5,0,45,0,0,0,5,5,5,10,10,10, 0,1,,0,)... ; Positioning, etc. N90 ; 2nd measurement CYCLE978(200,, ,1,77,2,8,1,1,1,"END_MILL_D8",,0,1.01,0.1,0.1,0.34,1,10001,,1,0)... ; Positioning, etc. N120 ; 3. measurement CYCLE998(100105,10004,0,1,1,1,,1,5,201,1,10,,,,,1,,1,) N140 M30 Log in tabular format "Tabular format" must be selected at "Log format" in the CYCLE150 screen form. This format can be imported into spreadsheet programs and processed further. The "Tabular format" is defined by the following default settings: Separation of the data fields: Decimal character: Date format: Number of decimal places: Time format: Semicolon Point yyyy-mm-dd As on the screen hh:mm:ss A log in tabular format contains the same information as in text format. For the statistical evaluation of measurement series, these logs require post processing in the respective spreadsheet programs User log Function With this function, the user freely defines the contents of the log lines and stores them in an array of string variables (string length 200). Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 65

64 Description 2.13 Miscellaneous functions The contents of the string array are logged when a new CYCLE160 is called. The logging always begins with array index 0 and continues until an empty string (i.e. string length 0) is found. For simple applications, an NCK-global array of string variables is predefined in the PGUD block: DEF NCK STRING[200] S_LOGTXT[10] This means that 10 lines can be immediately logged. If this is not sufficient, the user can alternatively create a second string array of any length with the predefined name S_USERTXT[n] in a separate GUD block (e.g. MGUD or UGUD): DEF NCK STRING[200] S_USERTXT[n] The logging function checks whether the S_USERTXT array is available. If it is available, the contents of this array are logged, if not, the contents of S_LOGTXT. At the program position where CYCLE160 is called, the logging is performed according to the logging destination set by the CYCLE150 call exactly the same as the logging of measurement results. This function can be used to output a complete user-specific log (without any reference to the measuring) or to insert additional lines in standard logs. If additional lines are to be written in standard logs in tabular format, the user must ensure the column formatting in these strings (insert separators ";"). Procedure "User log" is selected in the CYCLE150 screen form for the log control. There is no difference between text format and tabular format the user determines the contents. The corresponding selection field is hidden for the user log. If the path is entered, it is performed with the same dialog as for the standard log. 66 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

65 Description 2.13 Miscellaneous functions Image 2-15 User log screen form The following must be written in the part program: CYCLE150 call to activate the user log Assignment of the log contents to the predefined string variables CYCLE160 for the output of the log contents CYCLE160 has no transfer parameters. The user must program it without a screen form. Freely-definable user log Programming example:... N50 CYCLE150(10,1111, MY_PROT.TXT ) N51 S_USERTXT[0]=REP("") N52 S_USERTXT[0]="MACHINE: ABC_12345" ; Logging ON ; Delete old data array ; Compile log contents N53 S_USERTXT[1]="LOGFILE COMPENSATION DATA" N54 S_USERTXT[2]=" " N55 S_USERTXT[3]="VALUE1 = "<<R101 N56 S_USERTXT[4]="VALUE2 = "<<R102 N60 CYCLE160 ; Programming of empty line: 1 x blank ; Write user log Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 67

66 Description 2.13 Miscellaneous functions... M30 Log extract: MACHINE: ABC_12345 LOGFILE COMPENSATION DATA VALUE1 = VALUE2 = Explanations: N50 Logging is switched on Destination: In the same path as the calling program The log is appended Log type: User log Logging "on" N52 - N56 log content N60 CYCLE160 call: Data is now written Value 1 and value 2 mirror the contents of the R-parameters R101 and R102 at the time of the log output. Standard log with additional user data Programming example: --- N50 CYCLE150(10,1001, ) N51 S_LOGTXT[0]=REP("") N52 S_LOGTXT[0]="HOLE DM 20H7" N53 S_LOGTXT[1]="LARGESTDIMENSION: " N54 S_LOGTXT[2]="SMALLESTDIMENSION: " ; Logging ON, write header ; Delete old data array ; Write user data N55 S_LOGTXT[3]="SPINDLETEMPERATURE:"<<R99<<" DEG" N60 CYCLE160 T="3D_PROBE_FR" D1 M6 G0 X0 Y0 Z5 ; Write user data to log N70 CYCLE977(201,, ,1,24,,,2,8,0,1,1,,,1," ",, 0,1.01,1.01,-1.01,0.34,1,0,,1,1) 68 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

67 Description 2.13 Miscellaneous functions... M30 Log extract: ************************************************************************************************** Date : Time: 11:59:10 Protocol: /_N_WKS_DIR/_N_WP1_WPD/_PROT_TE_977_BOHR_TXT Program : _N_TE_977_BOHR_MPF Workpiece no.: 123 ************************************************************************************************* HOLE DM 20H7 LARGESTDIMENSION: SMALLESTDIMENSION: SPINDLETEMPERATURE:68.7 DEG : 977 / 101 Time: 11:58:10 Results measure: 1 Hole / CYCLE Correction into: Work offset, coarse G508 Coarse [mm] Rotation [deg] X Y Z Results: Setpoint Measured Difference X mm Y mm Diameter mm Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 69

68 Description 2.13 Miscellaneous functions Behavior during block search, simulation and for several channels Block search If during the block search, a cycle call for logging "On" is executed, this state is saved. The following measuring cycle calls that are run through in the block search mode do not log anything (because there are no measuring results). Logging is started as of the program start when the search target is reached. Similarly, the state is also saved for a cycle call for logging "Off" during the block search, and then nothing logged as of the program start. Simulation The following behavior applies in the simulation of Operate: Programs with calls for the logging function can be executed, but no logs are created. During simulation, measuring cycles do not return any measurement results, they only show the traversing to the measuring points and therefore there is nothing to log. Several channels In principle, measuring programs with logging can run in two channels. However, the user must ensure that the measuring and logging functions run in succession from channel to channel and do not overlap. This also applies to user logs. 70 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

69 3 3.1 General requirements Overview of the measuring cycles Function of the measuring cycles The following table describes all the measuring cycle functions for the turning and milling technologies. Table 3-1 Measuring cycle CYCLE973 2) CYCLE974 2) CYCLE994 2) CYCLE976 CYCLE961 CYCLE977 CYCLE978 Description This measuring cycle can be used to calibrate a workpiece probe on a surface on the workpiece or in a groove. This measuring cycle can be used to determine the workpiece zero in the selected measuring axis or a tool offset with 1-point measurement. This measuring cycle can be used to determine the workpiece zero in the selected measuring axis with 2-point measurement. To do this, two opposite measuring points on the diameter are approached automatically in succession Using this measuring cycle, a workpiece probe can be calibrated in a calibration ring or on a calibration ball completely in the working plane or at an edge for a particular axis and direction. This measuring cycle can be used to determine the position of a workpiece corner (inner or outer) and use this as work offset. This measuring cycle can be used to determine the center point in the plane as well as the width or the diameter. This measuring cycle can be used to measure the position of an edge in the workpiece coordinate system. Measuring versions Calibrate probe - length Calibrate probe - radius on surface Calibrate probe - probe in groove Turning measurement - front edge Turning measurement - inside diameter Turning measurement - outside diameter Turning measurement - inside diameter Turning measurement - outside diameter Calibrate probe - length on surface Calibrate probe - radius in ring Calibrate probe - radius on edge Calibrate probe - calibration on sphere Corner - right-angled corner Corner - any corner Edge distance - groove Edge distance - rib Hole - rectangular pocket Hole - 1 hole Spigot - rectangular spigot Spigot - 1 circular spigot Edge distance - set edge Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 71

70 3.1 General requirements Measuring cycle CYCLE979 CYCLE995 CYCLE996 CYCLE997 CYCLE998 CYCLE971 1) CYCLE982 2) Description This measuring cycle can be used to measure the center point in the plane and the radius of circle segments. With this measuring cycle the angularity of the spindle on a machine tool can be measured. This measuring cycle can be used to determine transformation-relevant data for kinematic transformations with contained rotary axes. This measuring cycle can be used to determine the center point and diameter of a ball. Furthermore, the center points of three distributed balls can be measured. The plane formed through the three ball center points, regarding its angular position, is determined referred to the working plane in the workpiece coordinate system. This measuring cycle can be used to determine the angular position of a surface (plane) referred to the working plane and the angle of edges in the workpiece coordinate system. This measuring cycle can be used to calibrate a tool probe and measure the tool length and/or tool radius for milling tools. This measuring cycle can be used to calibrate a tool probe and measure turning, drilling and milling tools on turning machines. Measuring versions Hole - inner circle segment Spigot - outer circle segment 3D - angular deviation spindle 3D - kinematics 3D - sphere 3D - 3 spheres Edge distance - align edge 3D - align plane Calibrate probe Measure tool Calibrate probe Turning tool Milling tool Drill 1) Only for milling technology 2) Only for turning technology 72 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

71 3.1 General requirements Selection of the measuring variants via softkeys (turning) The following shows the measuring variants of the turning technology as a menu tree in the program editor. Preconditions All of the measuring variants available in the control are shown in the display. However, on a specific system, only those steps can be selected that are possible for the set extended technology. 1) The "Inner diameter" softkey is displayed if bit1 =1 is set in the general SD $SNS_MEA_FUNCTION_MASK_TURN. 2) The "3D" softkey is displayed if bit 1 = 1 is set in the general SD $SNS_MEA_FUNC TION_MASK_PIECE. 3) The "kinematics" softkey is only displayed in the G code program if the "Measure kinematics" option is set. Turning technology menu tree (without extendable technology) These softkeys are displayed only when no extended technology is set (channel-specific MD52201 $MCS_TECHNOLOGY_EXTENSION = 0). See: "Measuring the workpiece on a machine with combined technologies (Page 229) ". Length (CYCLE973) (Page 209) Radius on surface (CYCLE973) (Page 82) Calibrate in groove (CYCLE973) (Page 85) Front edge (CYCLE974) (Page 91) Inner diameter (CYCLE974, CY CLE994) (Page 94) Outer diameter (CYCLE974, CY CLE994) (Page 99) Calibrate probe (CYCLE982) (Page 234) Turning tool (CYCLE982) (Page 239) Drill (CYCLE982) (Page 250) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 73

72 3.1 General requirements Turning technology with extended milling technology menu tree 4) The "Angular deviation spindle" softkey is exclusively displayed in the G code program. These softkeys are displayed if the "Milling" extended technology is set (channel-specific MD52201 $MCS_TECHNOLOGY_EXTENSION = 2). Length (CYCLE973) (Page 80) Radius in ring (CYCLE976) (Page 111) Radius at edge (CYCLE976) (Page 116) Calibrate on sphere (CYCLE976) (Page 122) Front edge (CYCLE974) (Page 91) 1) Inner diameter (CYCLE974, CY CLE994) (Page 94) Outer diameter (CYCLE974, CY CLE994) (Page 99) Set edge (CYCLE978) (Page 125) Align edge (CYCLE998) (Page 131) Groove (CYCLE977) (Page 138) Rib (CYCLE977) (Page 143) Right-angled corner (CYCLE961) (Page 148) Any corner (CYCLE961) (Page 153) Rectangular pocket (CYCLE977) (Page 158) 1 hole (CYCLE977) (Page 163) Inner circle segment (CYCLE979) (Page 168) Rectangular spigot (CYCLE977) (Page 173) 74 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

73 3.1 General requirements 1 circular spigot (CYCLE977) (Page 179) Outer circle segment (CYCLE979) (Page 184) 2) Align plane (CYCLE998) (Page 189) Sphere (CYCLE997) (Page 194) 3 spheres (CYCLE997) (Page 199) 4) Spindle angular displacement (CY CLE995) (Page 209) 3D kinematics (CYCLE996) (Page 209) Calibrate probe (CYCLE982) (Page 234) Turning tool (CYCLE982) (Page 239) Milling tool (CYCLE982) (Page 243) Drill (CYCLE982) (Page 250) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 75

74 3.1 General requirements Selection of the measuring variants via softkeys (milling) The following shows the measuring variants for the milling technology as a menu tree in the program editor. Requirements All of the measuring variants available in the control are shown in the display. However, on a specific system, only those steps can be selected that are possible for the set extended technology. 1) The "Inner diameter" softkey is displayed if bit1 =1 is set in the general SD $SNS_MEA_FUNCTION_MASK_TURN. 2) The "3D" softkey is displayed if bit 1 = 1 is set in the general SD $SNS_MEA_FUNC TION_MASK_PIECE. 3) The "Kinematics" softkey is only displayed in the G code program, if the "Measure kinematics" option is set. 4) The "Angular deviation spindle" softkey is exclusively displayed in the G code program. Milling technology menu tree Length (CYCLE976) Radius in ring (CYCLE976) (Page 111) Radius at edge (CYCLE976) (Page 116) Calibrate on sphere (CYCLE976) (Page 122) Set edge (CYCLE978) (Page 125) Align edge (CYCLE998) (Page 131) Groove (CYCLE977) (Page 138) Rib (CYCLE977) (Page 143) Right-angled corner (CYCLE961) (Page 148) Any corner (CYCLE961) (Page 153) Rectangular pocket (CYCLE977) (Page 158) 76 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

75 3.1 General requirements 1 hole (CYCLE977) (Page 163) Inner circle segment (CYCLE979) (Page 168) Rectangular spigot (CYCLE977) (Page 173) 1 circular spigot (CYCLE977) (Page 179) Outer circle segment (CYCLE979) (Page 184) 2) Align plane (CYCLE998) (Page 189) Sphere (CYCLE997) (Page 194) 3 spheres (CYCLE997) (Page 199) 4) Spindle angular displacement (CY CLE995) (Page 205) 4) Set front edge (CYCLE974) (Page 91) 1) Inner diameter (CYCLE974, CY CLE994) (Page 94) Outer diameter (CYCLE974, CY CLE994) (Page 99) Calibrate probe (CYCLE971) (Page 259) Measure tool (CYCLE971) See also Calibrate probe - calibrate in groove (CYCLE973) (Page 85) 3D - kinematics (CYCLE996) (Page 209) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 77

76 3.1 General requirements Result parameters Definition Result parameters are measurement results provided by the measuring cycles. Parameters Type Meaning _OVR[ ] REAL Result parameter - real number: Setpoint values, actual values, differences, offset values, etc. _OVI[ ] INTEGER Result parameter - integer Call The result parameters of the measuring cycles are saved in the channel-specific user variables. These can be called from the operating area as follows: 1. Press the "Parameter" softkey. 3. Press the "Using variable" softkey. The result parameters _OVR[ ] and _OVI[ ] are displayed in the "Channel-specific user variables" window. 2. Press the the "Channel GUD" softkey. Note If not only SGUD variables exist, the "GUD selection" softkey must be used to select "SGUD". Measuring versions Which result parameters are output from the measuring cycles, is described in the individual measuring versions. For workpiece measurement with tool offset or offset in the WO, several measuring versions also supply result parameters, see Chapter Additional result parameters (Page 321). 78 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

77 3.2 Measure workpiece (turning) 3.2 Measure workpiece (turning) General information The measuring cycles below are intended for use on turning machines. Note Spindle Spindle commands in the measuring cycles always refer to the active master spindle of the control. When using the measuring cycles at machines with several spindles, then the spindle involved must be defined as master spindle before the cycle call. Note Precise measurement is only possible with a probe calibrated under the measurement conditions, i.e. working plane and measuring velocity are the same for both measurement and calibration. If the probe is used in the spindle for a driven tool, the spindle orientation must also be considered. Deviations can cause measuring errors. References: /PG/ Programming Manual SINUMERIK 840D sl / 828D Fundamentals Diameter programming, measuring system The measuring cycles used in turning work with the current plane G18. Value specifications of the transverse axis (X) of the measuring cycles used in turning are performed in the diameter (DIAMON). The measuring cycles used in turning (CYCLE973, CYCLE974 and CYCLE994) also work internally with active diameter programming (DIAMON). The measuring system (basic system) of the machine and the workpiece can be different. The G700 command should be used when measuring the workpiece in INCHES on a metric machine. The G710 command should be used when measuring the workpiece in mm on an "INCH" machine. For information regarding measurement in conjunction with a 3rd axis, see Chapter Extended measurement (Page 105). Note A correspondence/assignment list of the measuring cycle parameters, machine and setting data used with regard to the measuring cycle versions 7.5, 2.6 and 4.4 can be found in the Appendix Changes from cycle version SW4.4 and higher (Page 325)! Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 79

78 3.2 Measure workpiece (turning) Calibrate probe - length (CYCLE973) Function Only applies on a turning machine without the milling technology. See "Measuring the workpiece on a machine with combined technologies (Page 229)". With this measuring version, a workpiece probe with cutting edge positions SL=5 to 8 can be calibrated on a known surface (workpiece-related). The trigger points of the probe are determined. Optionally, the actual length can be entered in the tool offset memory via the "Adapt tool length" parameter. Measuring principle The switching position of the workpiece probe in an axis is calculated into the measuring probe length. The calculated trigger point is determined in the corresponding axis and axis direction, and entered in the selected calibration data set (calibration data field) of the workpiece probe. The probe travels in the measuring direction to the calibration edge (e.g. workpiece) Image 3-1 Calibrate: Length on the surface (CYCLE973), example G18, SL=7 Requirements The surface must be in parallel to an axis of the workpiece coordinate system (WCS). The calibration surface must have a low surface roughness. The workpiece probe is called as tool with tool offset. 580 must be declared as the probe type. Starting position before the measurement The probe must be positioned opposite to the calibration surface. 80 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

79 3.2 Measure workpiece (turning) Position after the end of the measuring cycle The probe is at the distance of the selected measurement path (DFA) away from the calibration surface. Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Calibrate probe" softkey. 3. Press the "Length" softkey. The input window "Calibrate: Length at surface" opens. Parameters G code program ShopTurn program Parameters Description Unit Parameters Description Unit F Calibration data set (1-12) - T Name of the probe - Calibration and measuring feedrate Distance/ min D Cutting edge number (1-9) - β F Calibration data set (1-12) - Tool alignment with swivel axis (0 degrees) (90 degrees) Value entry Calibration and measuring feedrate Z Start point Z of the measurement mm X Start point X of the measurement mm Y Start point Y of the measurement mm Degrees mm/min Parameters Description Unit Adapt tool length Measuring direction Adapt the probe length and trigger point: Yes No (adapt trigger point only) Measuring axis (for G18): +/- Z +/- X Z0 / X0 Reference point Z/X (corresponding to the measuring direction) mm - - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 81

80 3.2 Measure workpiece (turning) Parameters Description Unit DFA Measurement path mm TSA Safe area for the measurement result mm Note When the calibration is performed for the first time, the default setting in the data field of the probe is still "0". For this reason, the TSA parameter must be programmed > probe ball radius to avoid the alarm "Safe area exceeded". List of the result parameters The measuring version "Length" provides the following result parameters: Table 3-2 "Length" result parameters Parameters Description Unit _OVR [4] Actual value probe ball diameter mm _OVR [5] Difference probe ball diameter mm _OVR [8] Trigger point in minus direction, actual value of 1st axis of the plane mm _OVR [10] Trigger point in plus direction, actual value of 1st axis of the plane mm _OVR [12] Trigger point in minus direction, actual value of 2nd axis of the plane mm _OVR [14] Trigger point in plus direction, actual value of 2nd axis of the plane mm _OVR [9] Trigger point in minus direction, difference of 1st axis of the plane mm _OVR [11] Trigger point in plus direction, difference of 1st axis of the plane mm _OVR [13] Trigger point in minus direction, difference of 2nd axis of the plane mm _OVR [15] Trigger point in plus direction, difference of 2nd axis of the plane mm _OVR [20] Positional deviation of the 1st axis of the plane (probe skew) mm _OVR [21] Positional deviation of the 2nd axis of the plane (probe skew) mm _OVR [27] Work offset range mm _OVR [28] Safe area mm _OVI [2] Measuring cycle number - _OVI [5] Probe number - _OVI [9] Alarm number Calibrate probe - radius on surface (CYCLE973) Function Only applies on turning machines without the milling technology. 82 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

81 3.2 Measure workpiece (turning) See "Measuring the workpiece on a machine with combined technologies (Page 229)". With this measuring version, the radius of a workpiece probe with cutting edge positions SL=5 to 8 can be calibrated on a surface. The trigger points of the probe are determined. The calibration surface is workpiece-related. It is only possible to calibrate in the selected axis and direction, which are perpendicular to this calibration surface. Measuring principle The determined switching position of the workpiece probe in the parameterized axis and direction, is calculated with the setpoint of the reference surface and from this the corresponding trigger point determined. If no alarms occur, the trigger values are entered into the selected calibration data set of the workpiece probe. The probe travels in the measuring direction to the reference surface (e.g. workpiece) Image 3-2 Calibrate: radius at the surface (CYCLE973), example G18, SL=8 Requirements The surface must be in parallel to an axis of the workpiece coordinate system (WCS). The calibration surface must have a low surface roughness. The workpiece probe is called as tool with tool offset. 580 must be declared as the probe type. Starting position before the measurement The probe must be positioned opposite to the calibration surface. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 83

82 3.2 Measure workpiece (turning) Position after the end of the measuring cycle The probe (ball radius) is the distance of the measurement path away from the calibration surface. Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Calibrate probe" softkey. 3. Press the "Radius on surface" softkey. The input window "Calibrate: Radius at surface" opens. Parameters G code program ShopTurn program Parameter Description Unit Parameter Description Unit F Calibration data set (1-12) - T Name of the probe - Calibration and measuring feedrate Distance/ min D Cutting edge number (1-9) - F β X Y Z Calibration data set (1-12) - Calibration and measuring feedrate Tool alignment with swivel axis (0 degrees) (90 degrees) Value entry Start point X of the measurement Start point Y of the measurement Start point Z of the measurement mm/min Degrees mm mm mm Parameters Description Unit Measuring direction Measuring axis (for measuring plane G18) - +/- Z +/- X Z0 / X0 Reference point Z/X (corresponding to the measuring direction) mm DFA Measurement path mm TSA Safe area for the measurement result mm 84 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

83 3.2 Measure workpiece (turning) Note When the calibration is performed for the first time, the default setting in the data field of the probe is still "0". For this reason, the TSA parameter must be programmed > probe ball radius to avoid the alarm "Safe area exceeded". List of the result parameters The measuring variant "Radius on surface" provides the following result parameters: Table 3-3 "Radius on surface" result parameters Parameters Description Unit _OVR [4] Actual value probe ball diameter mm _OVR [5] Difference probe ball diameter mm _OVR [8] Trigger point in minus direction, actual value of 1st axis of the plane mm _OVR [10] Trigger point in plus direction, actual value of 1st axis of the plane mm _OVR [12] Trigger point in minus direction, actual value of 2nd axis of the plane mm _OVR [14] Trigger point in plus direction, actual value of 2nd axis of the plane mm _OVR [9] Trigger point in minus direction, difference of 1st axis of the plane mm _OVR [11] Trigger point in plus direction, difference of 1st axis of the plane mm _OVR [13] Trigger point in minus direction, difference of 2nd axis of the plane mm _OVR [15] Trigger point in plus direction, difference of 2nd axis of the plane mm _OVR [20] Positional deviation of the 1st axis of the plane (probe skew) mm _OVR [21] Positional deviation of the 2nd axis of the plane (probe skew) mm _OVR [27] Zero offset area mm _OVR [28] Safe area mm _OVI [2] Measuring cycle number - _OVI [5] Probe number - _OVI [9] Alarm number Calibrate probe - calibrate in groove (CYCLE973) Function Only applies on turning machines without the milling technology. Using this measuring version, a workpiece probe with cutting edge position SL=7 or SL=8 can be calibrated in a reference groove machine-related in the axes of the plane. The measuring probe length or the probe sphere radius can be determined with the calibration. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 85

84 3.2 Measure workpiece (turning) With the radius determination, a calibration is possible in one direction or in opposite directions of an axis. It is also possible to determine the positional deviation (skew) of the probe and the effective diameter of the probe sphere during calibration in opposite directions. Measuring principle The measured switching positions of the workpiece probe in the parameterized axis are taken into account together with the machine-related data of the selected calibration groove. From this data, the trigger points are calculated in the positive and negative directions as well as the position deviation in this axis and the effective probe sphere diameter. The trigger points always refer to the center of the probe sphere (TCP). The probe moves in the selected measuring axis in both directions in the calibration groove. Calibrate: Probe in groove (CYCLE973), example G18, SL=7 Calibrate: Probe in groove (CYCLE973), example G18, SL=8 Requirements The workpiece probe must be called as tool with the associated tool offset. The machine-related geometrical dimensions of the selected calibration group must be saved before calibration in the corresponding general setting data. 86 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

85 3.2 Measure workpiece (turning) Geometry of the calibration groove, example G18, SL=7 Geometry of the calibration groove, example G18, SL=8 Table 3-4 General setting data for dimensions of the calibration groove Calibration groove General setting data KN_0 SD $SNS_MEA_CAL_EDGE_PLUS_DIR_AX2 KN_1 SD $SNS_MEA_CAL_EDGE_MI NUS_DIR_AX2 KN_2 SD $SNS_MEA_CAL_EDGE_BASE_AX1 KN_3 SD $SNS_MEA_CAL_EDGE_PLUS_DIR_AX1 KN_4 KN_5 SD $SNS_MEA_CAL_EDGE_MI NUS_DIR_AX1 SD $SNS_MEA_CAL_EDGE_UP PER_AX2 KN_6 SD $SNS_MEA_CAL_EDGE_BASE_AX2 Description Calibration groove edge in the positive direction of the 2nd measuring axis. Calibration groove edge in the negative direction of the 2nd measuring axis. Calibration groove base of the 1st measuring axis Calibration groove edge in the positive direction of the 1st measuring axis Calibration groove edge in the negative direction of the 1st measuring axis. Upper calibration groove edge of the 2nd measuring axis Calibration groove base of the 2nd measuring axis References: Commissioning Manual SINUMERIK Operate (IM9) / SINUMERIK 840D sl, Chapter "Measuring workpieces when turning". Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 87

86 3.2 Measure workpiece (turning) Starting position before the measurement The starting position should be selected so that the selected workpiece probe can be positioned in the shortest possible distance, collision-free, with paraxial movements, in the reference groove corresponding to the active cutting edge position. Position after the end of the measuring cycle When calibration with one calibration direction has been completed, the probe is positioned at the measurement distance (DFA) from the calibration surface. For calibration with two calibration directions, the probe is located at the start position after completion of the measuring operation. Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Calibrate probe" softkey. 3. Press the "Calibrate in groove" softkey. The input window "Calibrate: Probe in groove" opens. Parameter G code program ShopTurn program Parameter Description Unit Parameter Description Unit PL Measuring plane (G17 - G19) - T Name of the probe - F Calibration data set (1-12) - D Cutting edge number (1-9) - Calibration and measuring feedrate Distance/ min β F X Y Z Calibration data set (1-12) - Tool alignment with swivel axis (0 degrees) (90 degrees) Input value Calibration and measuring feedrate Start position X of the measurement Start position Y of the measurement Start position Z of the measurement Degrees mm/min mm mm mm 88 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

87 3.2 Measure workpiece (turning) Parameter Description Unit Calibrate Length (calibrate probe length) Calibration directions (only for "Radius" calibration) Measuring direction Adapt tool length (only for "Length" calibration) Calibration groove data set 1 Radius (calibrate probe radius) 1: Calibration in one direction 2: Calibration in opposite directions Measuring axis (corresponding to the measuring plane): (+/-) Z (+/-) X No (adapt trigger point only) Yes (adapt probe length and trigger point) 2 3 DFA Measurement path mm TSA Safe area for the measurement result mm Note When the calibration is performed for the first time, the default setting in the data field of the probe is still "0". For this reason, the TSA parameter must be programmed > probe sphere radius to avoid the alarm "Safe area exceeded". Measurement version, turning on a milling machine Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Calibrate probe" softkey. 3. Press the "Calibrate in groove" softkey. The input window "Calibrate: Probe in groove" opens. Parameter ShopMill program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Calibration data set (1-12) - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 89

88 3.2 Measure workpiece (turning) ShopMill program Parameter Description Unit β Tool alignment with swivel axis Degrees (0 degrees) (90 degrees) Input value F Calibration and measuring feedrate mm/min X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm List of the result parameters The measuring variant "Calibrate in groove" provides the following result parameters: Table 3-5 "Calibrate in groove" result parameters Parameters Description Unit _OVR [4] Actual value probe ball diameter mm _OVR [5] Difference probe ball diameter mm _OVR [8] Trigger point in minus direction, actual value of 1st axis of the plane mm _OVR [10] Trigger point in plus direction, actual value of 1st axis of the plane mm _OVR [12] Trigger point in minus direction, actual value of 2nd axis of the plane mm _OVR [14] Trigger point in plus direction, actual value of 2nd axis of the plane mm _OVR [9] Trigger point in minus direction, difference of 1st axis of the plane mm _OVR [11] Trigger point in plus direction, difference of 1st axis of the plane mm _OVR [13] Trigger point in minus direction, difference of 2nd axis of the plane mm _OVR [15] Trigger point in plus direction, difference of 2nd axis of the plane mm _OVR [20] Positional deviation of the 1st axis of the plane (probe skew) mm _OVR [21] Positional deviation of the 2nd axis of the plane (probe skew) mm _OVR [27] Work offset range mm _OVR [28] Safe area mm _OVI [2] Measuring cycle number - _OVI [5] Probe number - _OVI [9] Alarm number - 90 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

89 3.2 Measure workpiece (turning) Turning measurement - front edge (CYCLE974) Function With this measuring variant, workpiece dimensions can be measured at edges in the direction of the infeed axis and offsets derived from these. The measurement result and the measurement difference can be used for: Correction of a work offset Offset of a tool Measurement without offset Note Extended measurement Information on measurement in conjunction with a third axis can be found in ChapterExtended measurement (Page 105). Measuring principle The measuring cycle determines the actual value of a measuring point at an edge of the turned part, relative to the workpiece zero. The difference between the actual value (measured value) and a specified setpoint in the 1st axis of the plane is calculated (for G18: Z). An extended tool offset in the summed and setup offsets is possible. For the tool offset, generally empirical values can be included in the calculation. Image 3-3 Measure: Front edge (CYCLE974) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 91

90 3.2 Measure workpiece (turning) Requirements The probe must be calibrated in the measuring direction and active as tool. The probe type is 710 or 580. The cutting edge position can be 5 to 8 and must be suitable for the measurement task. If necessary, the workpiece must be positioned in the correct angular spindle position using spindle positioning (SPOS). Starting position before the measurement The probe must be positioned opposite to the surface/edge to be measured. Starting from this position, the measuring cycle always traverses the measuring axis in the direction of the setpoint. Position after the end of the measuring cycle When the measuring process has been completed, the probe is positioned at the distance of the measurement path (DFA) from the measuring surface. Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Turning measurement" softkey. 3. Press the "Set front edge" softkey. The input window "Measure: Front edge" opens. Parameter G code program ShopTurn program Parameter Description Unit Parameter Description Unit Calibration data set (1-12) - T Name of the probe - D Cutting edge number (1-9) - Calibration data set (1-12) - β Tool alignment with swivel axis Degrees (0 degrees) (90 degrees) Input value Z Start position Z of the measurement mm X Start position X of the measurement mm Y Start position Y of the measurement mm 92 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

91 3.2 Measure workpiece (turning) Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured values in an adjustable WO) 1) Tool offset (save measured value in the tool data) TR Name of tool to be corrected - D Cutting edge number of tool to be corrected - Z0 Reference point Z mm DFA Measurement path mm TSA Safe area for the measurement result mm Dimensional tolerance TUL TLL Use dimensional tolerance (only for the "Tool offset" correction target) Yes No Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") 1) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. - - mm mm Machine manufacturer Please observe the machine manufacturer s instructions. Measurement version, turning on a milling machine Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Turning measurement" softkey. 3. Press the "Set front edge" softkey. The input window "Measure: Front edge" opens. Parameter ShopMill program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Calibration data set (1-12) - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 93

92 3.2 Measure workpiece (turning) ShopMill program Parameter Description Unit β Tool alignment with swivel axis Degrees (0 degrees) (90 degrees) Input value Z Start position Z of the measurement mm X Start position X of the measurement mm Y Start position Y of the measurement mm List of the result parameters The measuring variant "Front edge" provides the following result parameters: Table 3-6 "Front edge" result parameters Parameters Description Unit _OVR [0] Setpoint value for measuring axis mm _OVR [1] Setpoint in 1st axis of the plane only for S_MA=1 mm _OVR [2] Setpoint in 2nd axis of the plane only for S_MA=2 mm _OVR [3] Setpoint in 3rd axis of the plane only for S_MA=3 mm _OVR [4] Actual value for measuring axis mm _OVR [5] Actual value in 1st axis of the plane only for S_MA=1 mm _OVR [6] Actual value in 2nd axis of the plane only for S_MA=2 mm _OVR [7] Actual value in 3rd axis of the plane only for S_MA=3 mm _OVR [16] Difference for measuring axis mm _OVR [17] Difference in 1st axis of the plane only for S_MA=1 mm _OVR [18] Difference in 2nd axis of the plane only for S_MA=2 mm _OVR [19] Difference in 3rd axis of the plane only for S_MA=3 mm _OVI [0] D number or WO number - _OVI [2] Measuring cycle number - For workpiece measurement with tool offset or correction in the work offset, additional parameters are displayed, seeadditional result parameters (Page 321) Turning measurement - inside diameter (CYCLE974, CYCLE994) Function With this measuring method, the inside diameter of cylindrical workpieces can be measured. The diameter and radius programming are supported. 94 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

93 3.2 Measure workpiece (turning) The measurement result (measurement difference) can be used for: Correction in the work offset (only for 1-point measurements) Offset of a tool Measurement without offset Note Extended measurement Information on measurement in conjunction with a third axis can be found in ChapterExtended measurement (Page 105). Measuring principle The measuring cycle determines the actual value of an inner diameter using a 1-point measurement or 2-point measurement symmetrically around the workpiece zero (center of rotation). The 2-point measurement is performed by reversing the spindle through 180 degrees of the workpiece or by making measurements above and below the center of rotation. An extended tool offset in the summed and setup offsets is possible. For the tool offset, generally empirical values can be included in the calculation. Image 3-4 Measure: Inside diameter (CYCLE974) Positioning "Travel below the center" (CYCLE994) For "Travel below the center", the inside diameter of the workpiece is measured using a 2-point measurement with the measuring cycle CYCLE994. Two opposite measuring points symmetrical to the workpiece zero (center of rotation) are approached at a distance of the setpoint specified by the user. A protection zone can be programmed, which should be taken into account when traversing. The user must take into account the ball radius of the probe when dimensioning the protection zone. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 95

94 3.2 Measure workpiece (turning) Image 3-5 Positions of the probe when measuring the inner diameter using 2-point measurement (CYCLE994) Measuring with reversal of the workpiece (CYCLE974) With this measuring method, the actual value of a workpiece with reference to the workpiece zero in the measuring axis is determined by acquiring two opposite points on the diameter. The workpiece is positioned by the cycle before the first measurement at the angular position programmed in parameter α0. After the 1st measurement, the cycle also automatically generates the 180 degrees reversal before the second measurement. The mean value is calculated from both measured values. A correction of the work offset (WO) is only possible when measuring without reversal (1-point measurement). Requirements The probe must be calibrated in the measuring direction. The probe of type 710 or 580 must be active. The cutting edge position can be 5 to 8 and must be suitable for the measurement task. Starting position before the measurement The probe should be positioned opposite the surface to be measured, above the turning center. Position after the end of the measuring cycle The probe is at a distance of the measuring path (DFA) from the measuring surface, above the turning center. When "Travel under the center of rotation" is selected, after the end of the measuring cycle, the probe is at a distance of the measuring path (DFA) from the measuring surface, below the center of rotation. 96 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

95 3.2 Measure workpiece (turning) Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Turning measurement" softkey. 3. Press the "Inside diameter" softkey. The input window "Measure: Inside diameter" opens. Parameter G code program ShopTurn program Parameter Description Unit Parameter Description Unit Calibration data set (1-12) - T Name of the probe - D Cutting edge number (1-9) - β Z X Calibration data set (1-12) - Tool alignment with swivel axis (0 degrees) (90 degrees) Input value Start position Z of the measurement Start position X of the measurement Degrees mm mm Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured value in an adjustable WO) Tool offset (save measured value in the tool data) TR Name of tool to be corrected - D Cutting edge number of tool to be corrected - Inner diameter mm Positioning Measuring without reversal of the workpiece - Measuring with reversal of the workpiece (180 ) 3) Travel below center (measuring above and below the center of rotation) α0 Starting angle for spindle reversal (only for positioning "with reversal") Degrees XR Retraction in X (diameter) mm ZR (for G18) Retraction in Z mm DFA Measurement path mm TSA Safe area for the measurement result mm 1) 2) - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 97

96 3.2 Measure workpiece (turning) Parameter Description Unit Dimensional tolerance TUL TLL Use dimensional tolerance (only for the "Tool offset" correction target) Yes No 1) Only for positioning "without reversal" Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") 2) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 3) The "Measurement with reversal of the workpiece" function is displayed if bit 0 is set in the general SD $SNS_MEA_FUNCTION_MASK_TURN. - mm mm Machine manufacturer Please observe the machine manufacturer s instructions. Measurement version, turning on a milling machine Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Turning measurement" softkey. 3. Press the "Set front edge" softkey. The input window "Measure: Front edge" opens. Parameter ShopMill program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Calibration data set (1-12) - β Tool alignment with swivel axis Degrees (0 degrees) (90 degrees) Input value Z Start position Z of the measurement mm X Start position X of the measurement mm 98 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

97 3.2 Measure workpiece (turning) List of the result parameters The measuring variant "Inside diameter" provides the following result parameters: Table 3-7 "Inside diameter" result parameters Parameters Description Unit _OVR [0] Diameter setpoint (note measuring axis S_MA) mm _OVR [1] Diameter setpoint in 1st axis of the plane only for S_MA=1 mm _OVR [2] Diameter setpoint in 2nd axis of the plane only for S_MA=2 mm _OVR [3] Diameter setpoint in 3rd axis of the plane only for S_MA=3 mm _OVR [4] Diameter actual value mm _OVR [5] Diameter actual value in 1st axis of the plane only for S_MA=1 mm _OVR [6] Diameter actual value in 2nd axis of the plane only for S_MA=2 mm _OVR [7] Diameter actual value in 3rd axis of the plane only for S_MA=3 mm _OVR [16] Diameter difference mm _OVR [17] Diameter difference in 1st axis of the plane only for S_MA=1 mm _OVR [18] Diameter difference in 2nd axis of the plane only for S_MA=2 mm _OVR [19] Diameter difference in 3rd axis of the plane only for S_MA=3 mm _OVI [0] D number - _OVI [2] Measuring cycle number - For workpiece measurement with tool offset or correction in the work offset, additional parameters are displayed, seeadditional result parameters (Page 321) Turning measurement - outside diameter (CYCLE974, CYCLE994) Function With this measuring method, the outer diameter of cylindrical workpieces can be measured. The diameter and radius programming are supported. The measurement result (measurement difference) can be used for: Correction in the work offset (only for measuring without reversal, 1-point measurement) Offset of a tool Measurement without offset Note Extended measurement Information on measurement in conjunction with a third axis can be found in ChapterExtended measurement (Page 105). Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 99

98 3.2 Measure workpiece (turning) Measuring principle The measuring cycle determines the actual value of an outer diameter using a 1-point measurement or 2-point measurement symmetrically around the workpiece zero (center of rotation). The 2-point measurement is performed by reversing the spindle through 180 degrees of the workpiece or by making measurements above and below the center of rotation. Measure: Outside diameter (CYCLE974) with/ without reversal of the workpiece Measure: Outside diameter (CYCLE994) above and below the turning center Positioning "Travel below the center" (CYCLE994) For "Travel below the center", the outer diameter of the workpiece is measured using a 2-point measurement with the measuring cycle CYCLE994. Two opposite measuring points symmetrical to the workpiece zero (center of rotation) are approached at a distance of the setpoint specified by the user. When traversing, a safety zone is taken into account. The user must take into account the ball radius of the probe when dimensioning the protection zone. 100 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

99 3.2 Measure workpiece (turning) Image 3-6 Positions of the probe when measuring the outer diameter (CYCLE994) with retraction path in X and Z Measuring with reversal of the workpiece (CYCLE974) With this measuring method, the actual value of a workpiece with reference to the workpiece zero in the measuring axis is determined by acquiring two opposite points on the diameter. The workpiece is positioned by the cycle before the first measurement at the angular position programmed in parameter α0. After the 1st measurement, the cycle also automatically generates the 180 degrees reversal before the second measurement. The mean value is calculated from both measured values. A correction of the work offset (WO) is only possible when measuring without reversal (1-point measurement). Preconditions The probe must be calibrated in the measuring directions. In the measuring method "Travel below the center of rotation", measurements can also be performed without previous calibration if bit 2 is set to 1 in the channel-specific MD $MCS_MEA_FUNCTION_MASK. The probe of type 710 or 580 must be active. The cutting edge position can be 5 to 8 and must be suitable for the measurement task. Starting position before the measurement The probe should be positioned opposite the surface to be measured, above the turning center. Position after the end of the measuring cycle The probe is at a distance of the measuring path (DFA) from the measuring surface, above the turning center. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 101

100 3.2 Measure workpiece (turning) If "Travel under the center of rotation" was selected, after the end of the measuring cycle, the probe is at a distance of the measuring path (DFA) from the measuring surface, below the center of rotation. Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Turning measurement" softkey. 3. Press the "Outside diameter" softkey. The input window "Measure: Outer diameter" opens. Parameter G code program ShopTurn program Parameter Description Unit Parameter Description Unit Calibration data set (1-12) - T Name of the probe - D Cutting edge number (1-9) - Calibration data set (1-12) - β Tool alignment with swivel axis Degrees (0 degrees) (90 degrees) Input value Z Start position Z of the measurement mm X Start position X of the measurement mm Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured value in an adjustable WO) Tool offset (save measured value in the tool data) TR Name of tool to be corrected - D Cutting edge number of tool to be corrected - Outer diameter mm Positioning Measuring without reversal of the workpiece - Measuring with reversal of the workpiece 3) Travel below center (measuring above and below the center of rotation) α0 Starting angle for spindle reversal (only for positioning "Measuring with reversal") Degrees ZR (for G18) Retraction in Z mm XR Retraction in X (in the diameter) mm 1) 2) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

101 3.2 Measure workpiece (turning) Parameter Description Unit DFA Measurement path mm TSA Safe area for the measurement result mm Dimensional tolerance TUL TLL Use dimensional tolerance (only for the "Tool offset" correction target) Yes No Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") 1) Only for positioning "Measuring without reversal" 2) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 3) The "Measurement with reversal of the workpiece" function is displayed if bit 0 is set in the general SD $SNS_MEA_FUNCTION_MASK_TURN. - mm mm Machine manufacturer Please observe the machine manufacturer s instructions. Measurement version, turning on a milling machine Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Turning measurement" softkey. 3. Press the "Outside diameter" softkey. The input window "Measure: Outer diameter" opens. Parameter ShopMill program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Calibration data set (1-12) - β Tool alignment with swivel axis Degrees (0 degrees) (90 degrees) Input value Z Start position Z of the measurement mm X Start position X of the measurement mm Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 103

102 3.2 Measure workpiece (turning) List of the result parameters The measuring variant "Outside diameter" provides the following result parameters: Table 3-8 "Outside diameter" result parameters Parameters Description Unit _OVR [0] Diameter setpoint (note measuring axis S_MA) mm _OVR [1] Diameter setpoint in 1st axis of the plane only for S_MA=1 mm _OVR [2] Diameter setpoint in 2nd axis of the plane only for S_MA=2 mm _OVR [3] Diameter setpoint in 3rd axis of the plane only for S_MA=3 mm _OVR [4] Diameter actual value mm _OVR [5] Diameter actual value in 1st axis of the plane only for S_MA=1 mm _OVR [6] Diameter actual value in 2nd axis of the plane only for S_MA=2 mm _OVR [7] Diameter actual value in 3rd axis of the plane only for S_MA=3 mm _OVR [16] Diameter difference mm _OVR [17] Diameter difference in 1st axis of the plane only for S_MA=1 mm _OVR [18] Diameter difference in 2nd axis of the plane only for S_MA=2 mm _OVR [19] Diameter difference in 3rd axis of the plane only for S_MA=3 mm _OVI [0] D number - _OVI [2] Measuring cycle number - For workpiece measurement with tool offset or correction in the work offset, additional parameters are displayed, seeadditional result parameters (Page 321). 104 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

103 Measuring variants 3.2 Measure workpiece (turning) Extended measurement Measuring in conjunction with a 3rd axis (Y) If a lathe has a 3rd axis, for technological reasons it can make sense to also use this as a measuring axis. In this case, pre-positioning and the measuring operation are realized in the 3rd axis (Y axis); however, the measuring result correction is entered in the tool and WO components of the 2nd geometry axis (X axis). The 3rd axis supports the radius and diameter programming according to the relationships of the 2nd geometry axis (X). Note The function of including the 3rd axis for lathes refers to the measuring cycles CYCLE974 and CYCLE994! This function must be enabled, see References: Commissioning Manual SINUMERIK Operate (IM9) / SINUMERIK 840D sl, Chapter "Measuring workpieces when turning". Extended bypass options for 2-point measurement (CYCLE994) If a lathe has a 3rd axis, then it can also be optionally used as a bypass axis. The bypass strategies discussed in the following can be realized using the parameter assignment screen forms or the number of the measuring axis (Parameter S_MA). Basis for the extended bypass strategy is that the 3rd axis has been enabled for measuring cycles. S_MA, multi-digit = 102 S_MA, multi-digit = Axis of the plane is the bypass axis (Z) 1. Axis of the plane is the bypass axis (Z) 2nd axis of the plane, is the measuring axis (X) 3rd axis is the measuring axis (Y) Probe with cutting edge position (SL)=7 Probe with SL=7 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 105

104 3.2 Measure workpiece (turning) S_MA, multi-digit = 302 S_MA, multi-digit = Axis is the bypass axis (Y) 2. Axis of the plane is the bypass axis (X) 2nd axis of the plane, is the measuring axis (X) 3rd axis is the measuring axis (Y) Probe with SL=7 Probe with SL=7 106 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

105 3.3 Measure workpiece (milling) 3.3 Measure workpiece (milling) General information Milling machines The measuring cycles below are intended for use on milling machines. Note Spindle Spindle commands in the measuring cycles always refer to the active master spindle of the control. When using the measuring cycles at machines with several spindles, then the spindle involved must be defined as master spindle before the cycle call. Note Precise measurement is only possible with a probe calibrated under the measurement conditions, i.e. working plane and measuring velocity are the same for both measurement and calibration. If the probe is used in the spindle for a driven tool, the spindle orientation must also be considered. Deviations can cause measuring errors. References: /PG/ Programming Manual SINUMERIK 840D sl / 828D Fundamentals Plane definition, measuring system The measuring cycles under milling work with the active planes G17, G18 or G19. The measuring system (basic system) of the machine and the workpiece can be different. The G700 command should be used when measuring the workpiece in INCHES on a metric machine. The G710 command should be used when measuring the workpiece in mm on an "INCH" machine. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 107

106 3.3 Measure workpiece (milling) Calibrate probe - length (CYCLE976) Function Function Using this measuring method, the length of a workpiece probe can be calibrated in the tool axis on a known surface (reference area). This can be done, for example, on a workpiece. Measuring principle The probe travels in the measuring direction on the edge (e.g. workpiece) Image 3-7 Calibrate: Length at edge (CYCLE976) The length of the probe is determined corresponding to the setting in general MD $MNS_MEA_FUNCTION_MASK, bit 1. The setting determines whether the tool length refers to the probe sphere center or the probe sphere circumference. In the "Tool length to sphere center" variant, a trigger value is entered in the calibration data according to the calibration direction. References: Commissioning Manual SINUMERIK Operate (IM9) / SINUMERIK 840D sl, Chapter " and measurement functions". 108 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

107 3.3 Measure workpiece (milling) Requirements The probe must be active as tool. Probe type: 3D multi probe (type 710) Mono probe (type 712) L probe (type 713) Note L probe application (type 713) Calibration in +Z (for towing measurement) is possible with the L probe. The basic alignment of the L probe boom is toward +X (offset angle = 0). If the probe boom is to be aligned in a different direction in the measuring program, this can be performed through a rotation around the tool axis (e.g. ROT Z = 90). The probe length must be known in the program for collision-free positioning of the workpiece probe and entered in the tool offset memory. The sphere radius must be known exactly and entered in the tool data. For example, this can be implemented using a previous calibration in the ring or on the sphere (valid for type 710, 712). The calibration surface is perpendicular to the measuring axis or tool axis. Starting position before the measurement The probe must be positioned opposite to the calibration surface. The distance between the probe and calibration surface should be approximately the same as the selected measurement path (DFA). Position after the end of the measuring cycle According to the measuring direction (X, Y, Z), the distance between the probe in AUTOMATIC operation and the calibration surface is the same as the distance of the selected measurement path (DFA). In JOG operation, the start position is approached again. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 109

108 3.3 Measure workpiece (milling) Calling the measuring version Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Calibrate probe" softkey. 3. Press the "Length" softkey. The input window "Calibrate: Length at edge" opens Parameters Parameters G code program ShopMill program Parameters Description Unit Parameters Description Unit PL Measuring plane (G17 - G19) - T Name of the probe - F Calibration data set (1-12) - D Cutting edge number (1-9) - Calibration and measuring feedrate Distance/ min F Calibration data set (1-12) - Calibration and measuring feedrate X Start point X of the measurement mm Y Start point Y of the measurement mm Z Start point Z of the measurement mm mm/min Parameters Description Unit Adapt tool length Yes (adapt probe length and trigger point) Measuring direction No (adapt trigger point only) Measuring axis (+/-) Z (for measuring plane G17) - Z0 Reference point Z (for measuring plane G17) mm DFA Measurement path mm TSA Safe area for the measurement result mm Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

109 3.3 Measure workpiece (milling) Note When the calibration is performed for the first time, the default setting in the data field of the probe is still "0". For this reason, the TSA parameter must be programmed > probe ball radius to avoid the alarm "Safe area exceeded" Result parameters List of the result parameters The measuring version "Length" provides the following result parameters: Table 3-9 "Length" result parameters Parameters Description Unit _OVR [4] Actual value probe ball diameter mm _OVR [5] Difference probe ball diameter mm _OVR [16] Trigger point in minus direction, actual value of 3rd axis of the plane mm _OVR [17] Trigger point in minus direction, difference of 3rd axis of the plane mm _OVR [18] Trigger point in plus direction, actual value of 3rd axis of the plane mm _OVR [19] Trigger point in plus direction, difference of 3rd axis of the plane mm _OVR [22] Probe length of the workpiece probe mm _OVR [27] Work offset range mm _OVR [28] Safe area mm _OVI [2] Measuring cycle number - _OVI [5] Probe number - _OVI [9] Alarm number Calibrate probe - radius in ring (CYCLE976) Function Using this measurement version, the following data can be calibrated: Inclined position of the workpiece probe Trigger values Radius of the probe in a calibration ring (in axes of the plane) The probe calibration in the ring can be on the basis of an unknown or known center point in the ring. With known center point, this corresponds to the starting position. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 111

110 3.3 Measure workpiece (milling) Calibration is also possible taking into account a starting angle when using the "Start at ring center" calibration method. Any obstacles in the measuring path or at the measuring point can be avoided when using a starting angle. Measuring principle Calibration always starts in the positive direction of the 1st axis of the actual machining plane. Eight calibration positions are to be acquired, divided into two passes. Depending on the probe type, the passes are made with a uniform spindle position or a reversal of 180 degrees. During the calibration process, the center point of the calibration ring (corresponding to the calibration method) and its distance to the starting position are determined. The calibration data / trigger values are significantly influenced in the result by the following variables: Physical probe ball radius Design of the probe Measuring velocity Calibration ring with corresponding accuracy Correct mounting of the calibrating ring Image 3-8 Calibrate: Radius in ring (CYCLE976) Preconditions The following requirements must be fulfilled for calibration in the ring: The probe must be active as tool. Probe type: 3D multi probe (type 710) Mono probe (type 712) Star-type probe (type 714) 112 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

111 3.3 Measure workpiece (milling) Note: The arms of a star-type probe (type 714) must be positioned at 90 degree angle to each other. The exact diameter of the calibration ring is known. Starting position before the measurement If the measuring cycle is not started at the center of the ring, the workpiece probe sphere center must be positioned close to the center of the ring as well as to a calibration height within the calibration ring. When starting the measuring cycle at the center of the ring, the workpiece probe sphere center must be positioned precisely at the ring center point as well as at a calibration height within the calibration ring. Position after the end of the measuring cycle When calibration is complete, the probe center is at calibration height in the center of the ring. Note For extremely high demands placed on the measuring accuracy, it makes sense to accept the distance between the center point and starting position in the work offset and to perform an additional calibration using this optimization. Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Calibrate probe" softkey. 3. Press the "Radius in ring" softkey. The input window "Calibrate: Radius in ring" opens. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 113

112 3.3 Measure workpiece (milling) Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit PL Measuring plane (G17 - G19) - T Name of the probe - F Calibration data set (1-12) - D Cutting edge number (1-9) - Calibration and measuring feedrate Distance/ min F X Y Z Calibration data set (1-12) - Calibration and measuring feedrate Start position X of the measurement Start position Y of the measurement Start position Z of the measurement mm/min mm mm mm Parameter Description Unit Ring diameter mm DFA Measurement path mm TSA Safe area for the measurement result mm Note When the calibration is performed for the first time, the default setting in the data field of the probe is still "0". For this reason, the TSA parameter must be programmed > probe ball radius to avoid the alarm "Safe area exceeded". Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Calibrate probe" softkey. 3. Press the "Radius in ring" softkey. The input window "Calibrate: Radius in ring" opens. 114 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

113 3.3 Measure workpiece (milling) Parameter ShopTurn program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - F X Y Z Calibration data set (1-12) - Calibration and measuring feedrate Start position X of the measurement Start position Y of the measurement Start position Z of the measurement mm/min mm mm mm List of the result parameters The measuring variant "Radius in Ring" provides the following result parameters: Table 3-10 "Radius in ring" result parameters Parameters Description Unit _OVR [4] Actual value probe ball diameter mm _OVR [5] Difference probe ball diameter mm _OVR [6] Center point of calibration ring in 1st axis of the plane mm _OVR [7] Center point of calibration ring in 2nd axis of the plane mm _OVR [8] Trigger point in minus direction, actual value of 1st axis of the plane mm _OVR [9] Trigger point in minus direction, difference of 1st axis of the plane mm _OVR [10] Trigger point in plus direction, actual value of 1st axis of the plane mm _OVR [11] Trigger point in plus direction, difference of 1st axis of the plane mm _OVR [12] Trigger point in minus direction, actual value of 2nd axis of the plane mm _OVR [13] Trigger point in minus direction, difference of 2nd axis of the plane mm _OVR [14] Trigger point in plus direction, actual value of 2nd axis of the plane mm _OVR [15] Trigger point in plus direction, difference of 2nd axis of the plane mm _OVR [20] Positional deviation of the 1st axis of the plane (probe skew) mm _OVR [21] Positional deviation of the 2nd axis of the plane (probe skew) mm _OVR [24] Angle at which the trigger points were determined Degrees _OVR [27] Zero offset area mm _OVR [28] Safe area mm _OVI [2] Measuring cycle number - _OVI [5] Probe number - _OVI [9] Alarm number - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 115

114 3.3 Measure workpiece (milling) Calibrate probe - radius on edge (CYCLE976) Function With this measuring method, a workpiece probe can be calibrated in an axis and the direction selected by the user at a reference surface perpendicular to this. This can be done, for example, on a workpiece. The determined trigger point is taken into the addressed calibration data field. Measuring principle The probe approaches the reference surface in the selected axis and direction. The determined calibration value (trigger point + position deviation) and probe ball radius are transferred into the addressed calibration data fields. Calibrate: Radius at edge (CYCLE976), calibration direction Preconditions The probe must be active as tool. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) Star-type probe (type 714) L probe (type 713) Starting position before the measurement The probe is positioned in the measuring height, approximately at the distance of the measurement path (DFA) opposite to the edge. 116 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

115 3.3 Measure workpiece (milling) Position after the end of the measuring cycle The probe ball center is located in front of the reference edge by the distance of the measuring path. Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Calibrate probe" softkey. 3. Press the "Radius at edge" softkey. The input window "Calibrate: Radius at edge" opens. Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit PL Measuring plane (G17 - G19) - T Name of the probe - F Calibration data set (1-12) - D Cutting edge number (1-9) - Calibration and measuring feedrate Distance/ min F X Y Z Calibration data set (1-12) - Calibration and measuring feedrate Start position X of the measurement Start position Y of the measurement Start position Z of the measurement mm/min mm mm mm Parameter Description Unit Calibration directions 1: Calibration in one direction - 2: Calibrations in opposite directions Measuring direction Measuring axis (for G17): - (+/-) X (+/-) Y DX /DY Distance between the edges (only for calibration directions "2") mm X0 / Y0 Reference point mm DFA Measurement path mm TSA Safe area for the measurement result mm Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 117

116 3.3 Measure workpiece (milling) Note When the calibration is performed for the first time, the default setting in the data field of the probe is still "0". For this reason, the TSA parameter must be programmed > probe ball radius to avoid the alarm "Safe area exceeded". List of the result parameters The measuring variant "Radius on edge" provides the following result parameters: Table 3-11 "Radius on edge" result parameters Parameters Description Unit _OVR [4] Actual value probe ball diameter mm _OVR [5] Difference probe ball diameter mm _OVR [8] Trigger point in minus direction, actual value of 1st axis of the plane mm _OVR [10] Trigger point in plus direction, actual value of 1st axis of the plane mm _OVR [12] Trigger point in minus direction, actual value of 2nd axis of the plane mm _OVR [14] Trigger point in plus direction, actual value of 2nd axis of the plane mm _OVR [9] Trigger point in minus direction, difference of 1st axis of the plane mm _OVR [11] Trigger point in plus direction, difference of 1st axis of the plane mm _OVR [13] Trigger point in minus direction, difference of 2nd axis of the plane mm _OVR [15] Trigger point in plus direction, difference of 2nd axis of the plane mm _OVR [20] Positional deviation of the 1st axis of the plane (probe skew) mm _OVR [21] Positional deviation of the 2nd axis of the plane (probe skew) mm _OVR [24] Angle at which the trigger points were determined Degrees _OVR [27] Zero offset area mm _OVR [28] Safe area mm _OVI [2] Measuring cycle number - _OVI [5] Probe number - _OVI [9] Alarm number Calibrate probe - radius between 2 edges (Cycle976) Function Function With this measuring version, a workpiece probe can be calibrated in an axis of the machining plane selected by the user, between two reference surfaces parallel to one another. 118 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

117 3.3 Measure workpiece (milling) Measuring principle The probe traverses with constant spindle alignment in the selected axis, between the reference surfaces. The traversing path must be at right angles to the reference surfaces. The determined calibration value (trigger point + position deviation) and probe ball radius are transferred into the addressed calibration data fields. Image 3-9 Calibrate: Radius between 2 edges (CYCLE976) Preconditions The probe must be active as tool. Tool type of the probe: 3D multi probe (type 710) Starting position before the measurement The probe must be positioned at the calibration height, approximately in the middle between the two edges. Position after the end of the measuring cycle The center of the probe is located in the middle between the two reference surfaces. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 119

118 3.3 Measure workpiece (milling) Calling the measuring version Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Calibrate probe" softkey. 3. Press the "Radius at edge" softkey. The input window "Calibrate: Radius at edge" opens. 4. In the selection field, Calibrate directions, select, "2". Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit PL Measuring plane (G17 - G19) - T Name of the probe - F Calibration data set (1-12) - D Cutting edge number (1-9) - Calibration and measuring feedrate Distance/ min F X Y Z Calibration data set (1-12) - Calibration and measuring feedrate Start position X of the measurement Start position Y of the measurement Start position Z of the measurement mm/min mm mm mm Parameter Description Unit Calibration directions 1: Calibration in one direction - 2: Calibrations in opposite directions Measuring direction Measuring axis (for G17): - (+/-) X (+/-) Y DX /DY Distance between the edges (only for calibration directions "2") mm X0 / Y0 Reference point mm DFA Measurement path mm TSA Safe area for the measurement result mm 120 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

119 3.3 Measure workpiece (milling) Note When the calibration is performed for the first time, the default setting in the data field of the probe is still "0". For this reason, the TSA parameter must be programmed > probe ball radius to avoid the alarm "Safe area exceeded" Result parameters List of the result parameters The measuring version "Radius between two edges" provides the following result parameters: Table 3-12 "Radius between two edges" result parameters Parameter Description Unit _OVR [4] Actual value probe ball diameter mm _OVR [5] Difference probe ball diameter mm _OVR [8] _OVR [10] _OVR [12] _OVR [14] _OVR [9] _OVR[11] _OVR[13] _OVR[15] Trigger point in minus direction, actual value of 1st axis of the plane Trigger point in plus direction, actual value of 1st axis of the plane Trigger point in minus direction, actual value of 2nd axis of the plane Trigger point in plus direction, actual value of 2nd axis of the plane Trigger point in minus direction, difference of 1st axis of the plane Trigger point in plus direction, difference of 1st axis of the plane Trigger point in minus direction, difference of 2nd axis of the plane Trigger point in plus direction, difference of 2nd axis of the plane _OVR[20] Positional deviation of the 1st axis of the plane (probe skew) mm _OVR[21] Positional deviation of the 2nd axis of the plane (probe skew) mm _OVR[27] Work offset range mm _OVR[28] Safe area mm _OVI[2] Measuring cycle number - OVI[5] Probe number - OVI[9] Alarm number - The result parameters are written to, which correspond to the selected axis. mm mm mm mm mm mm mm mm Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 121

120 3.3 Measure workpiece (milling) Calibrate probe - calibrate on ball (CYCLE976) Function Using this measuring method, a workpiece probe can be calibrated at any position in space. This has a special meaning in conjunction with swivel functions and transformations. The same calibration data is generated as for calibration in the ring: Inclined position of the workpiece probe Trigger values Radius of the probe ball In addition, the probe length in the tool axis can be determined based on the machine data. MD51740 $MNS_MEA_FUNCTION_MASK, Bit 1 (probe ball sensor or ball circumference) The calibration sphere center is determined as supplementary result. Measuring principle The measurement sequence is divided into the following steps: 1. Determining the center point coordinates of the reference sphere 2. Determining the calibration data This procedure can be made parallel to the axis by passing or moving around the reference sphere. Image 3-10 Calibration at the sphere (CYCLE976), example of overtravel (intermediate positioning parallel to the axis) Preconditions The diameter of the reference sphere must be known. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) 122 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

121 3.3 Measure workpiece (milling) Starting position before the measurement The workpiece probe must be positioned above the reference sphere so that it can be approached collision-free from above and at the circumference. Position after the end of the measuring cycle The workpiece probe is located above the sphere center. Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Calibrate probe" softkey. 3. Press the "Calibrate on ball" softkey. The input window "Calibrate: Probe on ball" opens. Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit PL Measuring plane (G17 - G19) - T Name of the probe - F Calibration data set (1-12) - D Cutting edge number (1-9) - Calibration and measuring feedrate Distance/ min F X Y Z Calibration data set (1-12) - Calibration and measuring feedrate Start position X of the measurement Start position Y of the measurement Start position Z of the measurement mm/min mm mm mm Parameter Description Unit Positioning Adapt tool length Moving around the sphere Parallel to the axis Moving around on a circular path Yes (adapt probe length and trigger point) No (adapt trigger point only) - - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 123

122 3.3 Measure workpiece (milling) Parameter Description Unit ZS (for G17) Upper edge of the calibration sphere (only for adapt tool length "Yes") mm Sphere diameter mm α0 Contact angle Degrees DFA Measurement path mm TSA Safe area for the measurement result mm Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Calibrate probe" softkey. 3. Press the "Calibrate on sphere" softkey. The input window "Calibration: Probe on sphere" opens. ShopTurn program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Calibration data set (1-12) - F Calibration and measuring feedrate mm/min X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm List of the result parameters The measuring variant "Radius on sphere" provides the following result parameters: Table 3-13 "Radius on sphere" result parameters Parameters Description Unit _OVR [4] Actual value probe ball diameter mm _OVR [5] Difference probe ball diameter mm _OVR [8] Trigger point in minus direction, actual value of 1st axis of the plane mm _OVR [10] Trigger point in plus direction, actual value of 1st axis of the plane mm _OVR [12] Trigger point in minus direction, actual value of 2nd axis of the plane mm 124 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

123 3.3 Measure workpiece (milling) Parameters Description Unit _OVR [14] Trigger point in plus direction, actual value of 2nd axis of the plane mm _OVR [16] Trigger point in minus direction, actual value of 3rd axis of the plane mm _OVR [18] Trigger point in plus direction, actual value of 3rd axis of the plane mm _OVR [9] Trigger point in minus direction, difference of 1st axis of the plane mm _OVR [11] Trigger point in plus direction, difference of 1st axis of the plane mm _OVR [13] Trigger point in minus direction, difference of 2nd axis of the plane mm _OVR [15] Trigger point in plus direction, difference of 2nd axis of the plane mm _OVR [17] Trigger point in minus direction, difference of 3rd axis of the plane mm _OVR [19] Trigger point in plus direction, difference of 3rd axis of the plane mm _OVR [20] Positional deviation of the 1st axis of the plane (probe skew) mm _OVR [21] Positional deviation of the 2nd axis of the plane (probe skew) mm _OVR [22] Probe length of the workpiece probe mm _OVR [24] Angle at which the trigger points were determined Degrees _OVR [27] Work offset range mm _OVR [28] Safe area mm _OVI [2] Measuring cycle number - _OVI [5] Probe number - _OVI [9] Alarm number Edge distance - set edge (CYCLE978) Function This measuring method determines the position of a paraxial edge in the workpiece coordinate system through 1-point measurement. When using probes with side boom (L probe, type 713), towing measurement is possible in the positive direction of the tool axis. With the "3D probe with spindle reversal" measuring method, measurement is performed in the axes of the plane as differential measurement. Two measurements are automatically carried out one after the other, one with a spindle position of 180 degrees, and one with 0 degrees. The special procedure for this measurement permits the use of an uncalibrated multidirectional probe. However, the correct tool radius of the probe must be determined once by calibrating the probe. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. With the "Align 3D probe" measuring method, the switching direction of the probe is always aligned to the current measuring direction. This function is recommended when high demands are placed on the measuring accuracy. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 125

124 3.3 Measure workpiece (milling) The measurement result (measurement difference) can be used as follows: Correction of a work offset Offset of a tool Measurement without offset Measuring principle The measuring cycle determines the actual value of a measuring point, taking into account the calibration values at one edge of the workpiece referred to its zero point. The difference between the actual value (measured value) and a specified setpoint in the parameterized measuring axis is calculated. Measure: Edge (CYCLE978) measuring direction: -X Measure: Edge (CYCLE978) measuring direction: +Z (towing measurement) 126 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

125 3.3 Measure workpiece (milling) Preconditions The probe must be active as tool. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) L probe (type 713) Note L probe application (type 713) Measurement in +Z (for towing measurement) is possible with the L probe. The basic alignment of the L probe boom is toward +X (offset angle = 0). If the probe boom is to be aligned in a different direction in the measuring program, this can performed through a rotation around the tool axis (e.g. ROT Z = 90). Star-type probe (type 714) When using the measuring version on lathes: Use probe type 710 or 580 Set the length reference of the workpiece probe to the center of the probe ball: MD51740 $MNS_MEA_FUNCTION_MASK, bit 1 = 0 Note The following measuring methods are only possible in the axes of the plane: 3D probe with spindle reversal (differential measurement) Align 3D probe The probe types 712, 713 and 714 generally cannot be used for these measuring methods. Starting position before the measurement The probe should be positioned at a distance that is somewhat greater than the measurement path (DFA) with respect to the surface to be measured. Position after the end of the measuring cycle After the measurement has been completed, the probe ball with its circumference is at a distance of the measuring path DFA with respect to the measuring surface. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 127

126 3.3 Measure workpiece (milling) Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Edge distance" softkey. 3. Press the "Set edge" softkey. The input window "Measure: Edge" opens. Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) PL Measuring plane (G17 - G19) - Measuring method Calibration data set (1-12) (only for measuring without spindle reversal) - T Name of the probe - D Cutting edge number (1-9) - Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) - Calibration data set (1-12) (only for measuring without spindle reversal) X Y Z Start position X of the measurement Start position Y of the measurement Start position Z of the measurement - - mm mm mm Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured value in a settable WO) 3) Tool offset (save measured value in the tool data) TR Name of tool to be corrected - D Cutting edge number of tool to be corrected Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

127 3.3 Measure workpiece (milling) Parameter Description Unit Measuring direction Measuring axis +/- X +/- Y +/- Z X0 / Y0 / Z0 Setpoint (corresponding to the measuring direction) mm DFA Measurement path mm TSA Safe area for the measurement result mm Dimensional tolerance TUL TLL Use dimensional tolerance for tool offset (only for the "Tool offset" correction target) Yes No Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") 1) The "3D probe with spindle reversal" function is shown if bit 16 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 2) The "Align 3D probe" function is shown if bit 17 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 3) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. - - mm mm Machine manufacturer Please observe the machine manufacturer s instructions. Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Edge distance" softkey. 3. Press the "Set edge" softkey. The input window "Measure: Edge" opens. Parameter ShopTurn program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 129

128 3.3 Measure workpiece (milling) ShopTurn program Parameter Description Unit Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) Calibration data set (1-12) (only for measuring without spindle reversal) X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm - - List of the result parameters The measuring variant "Set edge" provides the following result parameters: Table 3-14 "Set edge" result parameters Parameters Description Unit _OVR [0] Setpoint value for measuring axis mm _OVR [1] Setpoint in 1st axis of the plane only for S_MA=1 mm _OVR [2] Setpoint in 2nd axis of the plane only for S_MA=2 mm _OVR [3] Setpoint in 3rd axis of the plane only for S_MA=3 mm _OVR [4] Actual value for measuring axis mm _OVR [5] Actual value in 1st axis of the plane only for S_MA=1 mm _OVR [6] Actual value in 2nd axis of the plane only for S_MA=2 mm _OVR [7] Actual value in 3rd axis of the plane only for S_MA=3 mm _OVR [16] Difference for measuring axis mm _OVR [17] Difference in 1st axis of the plane only for S_MA=1 mm _OVR [18] Difference in 2nd axis of the plane only for S_MA=2 mm _OVR [19] Difference in 3rd axis of the plane only for S_MA=3 mm _OVR [21] Mean value mm _OVI [0] D number or WO number - _OVI [2] Measuring cycle number - _OVI [3] Measuring version - _OVS_TNAME Tool name - For workpiece measurement with tool offset or correction in the work offset, additional parameters are displayed, seeadditional result parameters (Page 321). 130 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

129 3.3 Measure workpiece (milling) Edge distance - align edge (CYCLE998) Function The workpiece lies in any direction, i.e. not parallel to the workpiece coordinate system (WCS) on the work table. By measuring two points on the workpiece reference edge that you have selected, you determine the angle to the active coordinate system. You can correct this angle as a rotation either in a geometry axis or as translational offset in a rotary axis (rotary table) in any WO or in the active WO. Note Maximum measured angle Using the "Align edge" measuring version, a maximum angle of +/- 45 degrees can be measured. Measuring principle The Align edge measuring variant is performed according to the 1-angle measurement principle: For a clamped workpiece that is rotated in the plane, the angular offset is in the rotary part of the geometry axis that is located perpendicular to the measuring plane. Example of G17 plane: Measuring axis X, offset axis Y Angular offset is realized in the Z rotation The rotation offset in the WO is performed so that the actual position of the edge (actual value) and the desired setpoint angle (α) in the workpiece coordinate system must be taken into account. For a workpiece on a rotary table, the angular offset is added to the translatory offset of the rotary axis (table axis). The correction only makes sense if the rotary axis rotates around the geometry axis that is located perpendicular to the measuring plane. Example of G17 plane: Measuring axis X, offset axis Y Angular offset is realized in the C axis. Rotary axis C rotates a rotary table around the Z axis. After the measurement, the rotary axis should be repositioned to align the workpiece. Example: G55 G0 C0. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 131

130 3.3 Measure workpiece (milling) For both correction versions, the translational components the WO remain unchanged and should be redetermined after the edge has been aligned. This can be realized in a subsequent measuring program using the function "Set edge". Measure: Align edge (CYCLE998), workpiece clamped in the plane Measuring without spindle reversal Measure: Align edge (CYCLE998), workpiece clamped on rotary table C axis Precise measurement is only possible with a calibrated probe, i.e. machining plane, orientation of the spindle in the plane and measuring velocity are the same for both measurement and calibration. Deviations can cause additional measuring errors. Measuring with spindle reversal With measuring method "3D probe with spindle reversal", measuring point P1 is measured twice each with 180 degrees spindle reversal (probe rotated through 180 degrees) and 0 degrees. This means that the trigger points for the corresponding axis direction are currently being newly determined for this measurement (it is not necessary to calibrate the probe in the measuring direction). The measuring method "3D probe with spindle reversal" only makes sense for align edge of the axes in the working plane (for G17 XY). The special procedure for this measurement permits the use of an uncalibrated multidirectional probe. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. Preconditions The probe must be called as a tool with a tool length compensation. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) 132 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

131 3.3 Measure workpiece (milling) Note Precisely determining the angle requires the corresponding surface quality at least at one of the measuring points. The distances between the measuring points should be selected as high as possible. Note The "3D probe with spindle reversal" function (differential measurement) is only possible in the axes of the plane. The probe types 712, 713 and 714 generally cannot be used for this measuring method. Starting position before the measurement Measuring axis and positioning axis (offset axis) can be preselected as required; however, they may not be the same. Positioning taking into account a protection zone Protection zone = no The probe is positioned in the measuring axis, as a maximum at the distance of measurement path DFA with respect to the surface to be measured in front of measuring point P1 at the measuring height. Protection zone = yes The probe is positioned in the measuring axis as a maximum the distance from the measuring path DFA and the absolute value in parameter DX (for G17 and measuring axis X) with respect to the surface to be measured in front of measuring point P1 at the measuring height. In both cases, when making the measurement, measuring point P1 must be able to be safely reached. For the 1st measurement, if the distances from the reference edge are selected to be too large, then a measurement is not made. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 133

132 3.3 Measure workpiece (milling) Intermediate positioning from measuring point P1 to measuring point P2 Intermediate positioning "parallel to the edge" Image 3-11 Aligning the edge (CYCLE998), intermediate positioning "parallel to the edge" The probe travels parallel to the reference edge at the distance of parameter L2 in front of measuring point P2. In so doing, the angle from parameters α and TSA is taken into account. TSA contains the value for the maximum permissible angular deviation. Intermediate positioning "parallel to the axis" Image 3-12 Aligning the edge (CYCLE998), intermediate positioning "parallel to the axis" The probe travels parallel to the positioning axis (offset axis) at a distance of parameter L2 in front of measuring point P2. Position after the end of the measuring cycle After the end of measurement, the probe is at measuring point P2 at the distance of the measurement path DFA with respect to the measuring surface. 134 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

133 3.3 Measure workpiece (milling) Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Edge distance" softkey. 3. Press the "Align edge" softkey. The input window "Measure: Align edge" opens. Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit Measuring method Standard measuring method 3D probe with spindle reversal 1) PL Measuring plane (G17 - G19) - Measuring method Calibration data set (1-12) (only for standard measuring method) - T Name of the probe - D Cutting edge number (1-9) - Standard measuring method 3D probe with spindle reversal 1) - Calibration data set (1-12) (only for standard measuring method) X Y Z Start position X of the measurement Start position Y of the measurement Start position Z of the measurement - - mm mm mm Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured values in a settable WO) 2) - Angular offset (only for "work offset") Positioning Offset results in: Coordinate system rotation Rotary axis rotation C 3) Position probe: Parallel to the axis Parallel to the edge - - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 135

134 3.3 Measure workpiece (milling) Parameter Description Unit Measuring direction Positioning axis Measuring axis (+/-) X (+/-) Y (+/-) Z Offset axis (Note: Measuring axis and offset axis may not be the same!) X Y Z α Angle between positioning axis and edge 4) Degrees L2 Distance to the 2nd measuring point 5) mm Protection zone DX / DY / DZ (corresponding to the measuring direction) Use protection zone Yes No Distance to the edge for measuring point 1 (only for protection zone "Yes") DFA Measurement path mm TSA Safe area for the measurement result Degrees 1) The "3D probe with spindle reversal" function is shown if bit 16 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 2) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 3) To display the corresponding rotary axis as offset target, bit 6 must be set to 1 in the channel-specific MD $MCS_AXIS_USAGE_ATTRIB. If the offset (correction) involves more than one rotation around one of the geometry axes, then this offset cannot be executed by a rotary axis. Alarm "Correction of the work offset not executed" is output. 4) By specifying the measuring axis in parameter measuring direction, then all three measuring planes are possible. Setpoint angle α therefore refers to the positive direction of the offset axis and is negative in the clockwise sense, positive in the counter-clockwise sense. Setpoint angle α specifies the required angle between the edge and the positive direction of the offset axis. For α=0 (S_STA=0), after correction, regarding the offset axis, the edge is parallel to the axis. When positioning "Parallel to the edge", angle α is also used for positioning. The positioning angle is generated together with parameter TSA. Parameter α should therefore only deviate a small amount from the measured angle! 5) With parameter L2 (S_ID) the distance in the offset axis between P1 and P2 is defined. Only positive values are permissible for L2. Accordingly, P1 should be selected in the offset axis at the beginning of the cycle mm Machine manufacturer Please observe the machine manufacturer s instructions. 136 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

135 3.3 Measure workpiece (milling) Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Edge distance" softkey. Parameter ShopTurn program 3. Press the "Align edge" softkey. The input window "Measure: Align edge" opens. Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Measuring method Standard measuring method 3D probe with spindle reversal 1) - Calibration data set (1-12) (only for standard measuring method) X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm - List of the result parameters The measuring variant "Align edge" provides the following result parameters: Table 3-15 "Align edge" result parameters Parameters Description Unit _OVR [0] Angle setpoint Degrees _OVR [4] Angle actual value Degrees _OVR [16] Angle difference Degrees _OVR [20] Angle offset value Degrees _OVR [28] Safe area Degrees _OVR [30] Empirical value Degrees _OVI [0] WO number - _OVI [2] Measuring cycle number - _OVI [5] Probe number - _OVI [7] Empirical value memory number - _OVI [9] Alarm number - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 137

136 3.3 Measure workpiece (milling) Edge distance - groove (CYCLE977) Function This measuring version can be used to measure a groove in a workpiece. The groove width is measured and the groove center point determined. Measurements at an inclined groove are also possible. To do this, an angle corresponding to the actual angularity of the groove position should be entered into the parameterizing screen form. Probing at the groove edge always takes place at right angles. A protection zone can be defined in the groove. With the "3D probe with spindle reversal" measuring method, measurement is performed in the axes of the plane as differential measurement. Two complete measurements of the groove are automatically carried out one after the other, one with a spindle position of 180 degrees, and one with 0 degrees. The special procedure for this measurement permits the use of an uncalibrated multi-directional probe. However, the correct tool radius of the probe must be determined once by calibrating the probe. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. With the "Align 3D probe" measuring method, the switching direction of the probe is always aligned to the current measuring direction. This function is recommended when high demands are placed on the measuring accuracy. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. The measurement result (measurement difference) can be used as follows: Correction of a WO so that the workpiece zero point is in relation to the groove center point. Offset of a tool Measurement without offset Measuring principle One point at each of the opposite edges of the slot are measured based on the selected measuring axis. The positive direction of the geometry axis is measured first. From the two actual positions, taking into account the calibration values, the groove width is calculated. The position of the groove center as workpiece zero is determined corresponding to the work offset selected to be corrected. 138 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

137 3.3 Measure workpiece (milling) The measured difference of the groove width is used as basic variable for a tool offset, the position of groove zero point, as basis of a work offset. Measure: Groove (CYCLE977) Measure: Groove with protection zone (CY CLE977) Preconditions The probe must be active as tool. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) Note The following measuring methods are only possible in the axes of the plane: 3D probe with spindle reversal (differential measurement) Align 3D probe The probe types 712, 713 and 714 generally cannot be used for these measuring methods. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 139

138 3.3 Measure workpiece (milling) Starting position before the measurement The probe should be positioned with the probe ball center in the measuring axis approximately at the center of the groove and at the measuring height. For a protection zone, the probe ball should be positioned in the measuring axis approximately centered to the groove and at a height above the protection zone. With the infeed path that has been entered, it must be guaranteed that from this height the desired measuring height in the groove can be reached. Note If too large a measurement path DFA has been selected so that the protection zone is violated, then the distance is reduced automatically in the cycle. However, there must be sufficient room for the probe ball. Position after the end of the measuring cycle Without activated protection zone, the probe ball is at the measuring height in the center of the groove. With protection zone, the probe ball is centered with respect to the groove over the protection zone at the starting position of the measuring cycles. Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Edge distance" softkey. 3. Press the "Groove" softkey. The input window "Measure: Groove" opens. 140 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

139 3.3 Measure workpiece (milling) Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) PL Measuring plane (G17 - G19) - Measuring method Calibration data set (1-12) (only for measuring without spindle reversal) - T Name of the probe - D Cutting edge number (1-9) - Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) - Calibration data set (1-12) (only for measuring without spindle reversal) X Y Z Start position X of the measurement Start position Y of the measurement Start position Z of the measurement - - mm mm mm Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured values in an adjustable WO) 3) Tool offset (save measured values in the tool data) TR Name of tool to be corrected - D Cutting edge number of tool to be corrected - Measuring axis Measuring axis (for G17): X Y W Groove width setpoint mm α0 Angle between measuring axis and workpiece Degrees Protection zone Use protection zone Yes No only for protection zone "Yes": WS Width of the protection zone mm DZ Infeed distance at measuring height (for G17) mm DFA Measurement path mm TSA Safe area for the measurement result mm Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 141

140 3.3 Measure workpiece (milling) Parameter Description Unit Dimensional tolerance TUL TLL Use dimensional tolerance for tool offset (only for the "Tool offset" correction target) Yes No Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") 1) The "3D probe with spindle reversal" function is shown if bit 16 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 2) The "Align 3D probe" function is shown if bit 17 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 3) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. - mm mm Machine manufacturer Please observe the machine manufacturer s instructions. Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Edge distance" softkey. Parameter ShopTurn program 3. Press the "Groove" softkey. The input window "Measure: Groove" opens. Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) Calibration data set (1-12) (only for measuring without spindle reversal) X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

141 3.3 Measure workpiece (milling) List of the result parameters The measuring variant "Groove" provides the following result parameters: Table 3-16 "Groove" result parameters Parameters Description Unit _OVR [0] Groove width setpoint mm _OVR [1] Setpoint, groove center in the 1st axis of the plane mm _OVR [2] Setpoint, groove center in the 2nd axis of the plane mm _OVR [4] Groove width actual value mm _OVR [5] Actual value, groove center in the 1st axis of the plane mm _OVR [6] Actual value, groove center in the 2nd axis of the plane mm _OVR [16] Groove width difference mm _OVR [17] Difference, groove center in the 1st axis of the plane mm _OVR [18] Difference, groove center in the 2nd axis of the plane mm _OVI [0] D number or WO number - _OVI [2] Measuring cycle number - _OVI [3] Measuring version - _OVS_TNAME Tool name - For workpiece measurement with tool offset or correction in the work offset, additional parameters are displayed, seeadditional result parameters (Page 321) Edge distance - rib (CYCLE977) Function This measuring variant can be used to measure a rib on a workpiece. The rib width is measured and the rib center point is determined. Measurements at an inclined rib are also possible. To do this, an angle corresponding to the actual angularity of the rib position should be entered into the parameterizing screen form. Probing at the rib edge always takes place at right angles. A protection zone can be defined at the side of the rib. With the "3D probe with spindle reversal" measuring method, measurement is performed in the axes of the plane as differential measurement. Two complete measurements of the rib are automatically carried out one after the other, one with a spindle position of 180 degrees, and one with 0 degrees. The special procedure for this measurement permits the use of an uncalibrated multi-directional probe. However, the correct tool radius of the probe must be determined once by calibrating the probe. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. With the "Align 3D probe" measuring method, the switching direction of the probe is always aligned to the current measuring direction. This function is recommended when high demands Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 143

142 3.3 Measure workpiece (milling) are placed on the measuring accuracy. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. The measurement result (measurement difference) can be used as follows: Correction of a WO so that the workpiece zero point is in relation to the rib center point. Offset of a tool Measurement without offset Measuring principle One point at each of the opposite edges of the rib are measured based on the selected measuring axis. The positive direction of the geometry axis is measured first. From the two actual positions, taking into account the calibration values, the rib width is calculated. The position of the rib center as workpiece zero is determined corresponding to the work offset selected to be corrected. The measured difference of the rib width is used as basic variable for a tool offset, the position of rib zero point, as basis of a work offset. Measure: Rib (CYCLE977) Measure: Rib with a protection zone (CY CLE977) Preconditions The probe must be active as tool. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) 144 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

143 3.3 Measure workpiece (milling) Note The following measuring methods are only possible in the axes of the plane: 3D probe with spindle reversal (differential measurement) Align 3D probe The probe types 712, 713 and 714 generally cannot be used for these measuring methods. Starting position before the measurement The probe should be positioned with the probe ball center in the measuring axis approximately above the center of the rib. With the entered infeed path, it must be ensured that from the starting height the required measuring height at the rib is reached. Note If too large a measurement path DFA has been selected so that the protection zone is violated, then the distance is reduced automatically in the cycle. However, there must be sufficient room for the probe ball. Position after the end of the measuring cycle The probe ball is centered above the rib at the height of the starting position of the measuring cycles. Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Edge distance" softkey. 3. Press the "Rib" softkey. The input window "Measure: Rib" opens. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 145

144 3.3 Measure workpiece (milling) Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) PL Measuring plane (G17 - G19) - Measuring method Calibration data set (1-12) (only for measuring without spindle reversal) - T Name of the probe - D Cutting edge number (1-9) - Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) - Calibration data set (1-12) (only for measuring without spindle reversal) X Y Z Start position X of the measurement Start position Y of the measurement Start position Z of the measurement - - mm mm mm Parameter Description Unit Correction target Measuring only (no offset) - Work offset (save measured values in an adjustable WO) 3) Tool offset (save measured values in the tool data) TR Name of tool to be corrected - D Cutting edge number of tool to be corrected - Measuring axis Measuring axis (for measuring plane G17) - X Y W Rib width setpoint mm α0 Angle between measuring axis and workpiece Degrees DZ Infeed distance at measuring height (for measuring plane G17) mm Protection zone Use protection zone - Yes No WS Width of the protection zone (only for protection zone "Yes") mm DFA Measurement path mm TSA Safe area for the measurement result mm 146 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

145 3.3 Measure workpiece (milling) Parameter Description Unit Dimensional tolerance TUL TLL Use dimensional tolerance for tool offset Yes No Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") 1) The "3D probe with spindle reversal" function is shown if bit 16 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 2) The "Align 3D probe" function is shown if bit 17 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 3) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. - mm mm Machine manufacturer Please observe the machine manufacturer s instructions. Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Edge distance" softkey. Parameter ShopTurn program 3. Press the "Rib" softkey. The input window "Measure: Rib" opens. Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) Calibration data set (1-12) (only for measuring without spindle reversal) X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm - - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 147

146 3.3 Measure workpiece (milling) List of the result parameters The measuring variant "Rib" provides the following result parameters: Table 3-17 "Rib" result parameters Parameters Description Unit _OVR [0] Rib width setpoint mm _OVR [1] Rib center setpoint in the 1st axis of the plane mm _OVR [2] Rib center setpoint in the 2nd axis of the plane mm _OVR [4] Rib width actual value mm _OVR [5] Rib center actual value in the 1st axis of the plane mm _OVR [6] Rib center actual value in the 2nd axis of the plane mm _OVR [16] Rib width difference mm _OVR [17] Rib center difference in the 1st axis of the plane mm _OVR [18] Rib center difference in the 2nd axis of the plane mm _OVI [0] D number or WO number - _OVI [2] Measuring cycle number - _OVI [3] Measuring version - _OVS_TNAME Tool name - For workpiece measurement with tool offset or correction in the work offset, additional parameters are displayed, seeadditional result parameters (Page 321) Corner - right-angled corner (CYCLE961) Function This measuring variant can be used to measure a right-angled inside or outside corner of a workpiece. The measurements are performed paraxially to the active workpiece coordinate system. In addition to the measurement, the position of the corner can be used as workpiece zero in a specified zero offset (ZO). Measuring principle The measuring cycle moves to three measuring points and determines the point of intersection of the resulting straight lines and the angle of rotation to the positive 1st axis of the actual plane. The corner to be calculated can be offset. The result, the position of the corner is saved as an absolute value in the result parameters _OVR[ ] and optionally in the specified zero offset (offset and rotation). The measured corner 148 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

147 3.3 Measure workpiece (milling) is shifted by the values in setpoint parameter (X0, Y0 for G17) in the workpiece coordinate system in the plane. Measure: Right-angled corner, inner (CY CLE961) Measure: Right-angled corner, outer (CY CLE961) Requirements The probe must be called as a tool with a tool length compensation. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) Starting position before the measurement The probe is at the measuring height or above the corner (see protection zone) compared to the corner to be measured or in front of the 1st measuring point. The measuring points must be able to be approached from here collision-free. The measuring points are derived from the programmed distances L1 to L3 and the pole position (XP, YP). When positioning, α0 (angle between the X axis and 1st edge in the machine coordinate system) is also taken into account. The measuring cycle generates the required traversing blocks and performs the measurements at the measuring points P1 to P3, starting with P1. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 149

148 3.3 Measure workpiece (milling) Positioning measuring points P1 to P3 taking into account a protection zone Protection zone = no The probe is pre-positioned at the measuring height and remains at this measuring height when measuring the corner. An outer corner is traversed around. Protection zone = yes The probe is pre-positioned above the corner. When measuring, the 3rd axis of the plane (Z for G17) is moved by the value in parameter DZ to the measuring height and the corresponding measuring point is measured. After the measurement, the probe is raised by the value of parameter DZ and moves to the next measuring point, where it is lowered again. Image 3-13 Protection zone = yes Traversing around the outer corner with DZ>0 (measuring height + DZ) for G17 Position after the end of the measuring cycle The probe is at the starting position again (opposite the measured corner). Depending on the protection zone parameter yes/no, the probe is at the measuring height or above the corner. Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Corner" softkey. 3. Press the "Right-angled corner" softkey. The input window "Measure: Right-angled corner" opens. 150 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

149 3.3 Measure workpiece (milling) Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit PL Measuring plane (G17 - G19) - T Name of the probe - Calibration data set (1-12) - D Cutting edge number (1-9) - X Y Z Calibration data set (1-12) - Start position X of the measurement Start position Y of the measurement Start position Z of the measurement mm mm mm Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured values in an adjustable WO) 1) - Position Type of corner: - Position of the corner Outside corner Inside corner - X0 Setpoint X of the corner (for measuring plane G17) mm Y0 Setpoint Y of the corner (for measuring plane G17) mm XP Pole (for measuring plane G17) mm YP Pole (for measuring plane G17) mm α0 Angle between Y or Z axis and the 1st edge (for measuring plane G17) Degrees L1 L2 L3 Protection zone Distance between the pole and measuring point P1 in the direction of the 1st axis of the plane (for G17, X) Distance between the pole and measuring point P2 in the direction of the 1st axis of the plane Distance between the pole and measuring point P3 in the direction of the 2nd axis of the plane (for G17, Y) Use protection zone Yes No DZ Infeed distance at measuring height (only for protection zone "Yes") mm DFA Measurement path mm TSA Safe area for the measurement result mm 1) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. - mm mm mm - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 151

150 3.3 Measure workpiece (milling) Machine manufacturer Please observe the machine manufacturer s instructions. Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Corner" softkey. 3. Press the "Right-angled corner" softkey. The input window "Measure: Right-angled corner" opens. Parameter ShopTurn program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Calibration data set (1-12) - X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm List of the result parameters The measuring variant "Right-angled corner" provides the following result parameters: Table 3-18 "Right-angled corner" result parameters Parameters Description Unit _OVR [4] Angle actual value to the 1st axis of the plane in the workpiece coordinate system (WCS) _OVR [5] Corner point actual value in the 1st axis of the plane in the WCS mm _OVR [6] Corner point actual value in the 2nd axis of the plane in the WCS mm _OVR [20] Angle actual value to the 1st axis of plane in the machine coordinate system (MCS) 1) _OVR [21] Corner point actual value in the 1st axis of the plane in the MCS 1) mm _OVR [22] Corner point actual value in the 2nd axis of the plane in the MCS 1) mm _OVI [2] Measuring cycle number - _OVI [3] Measuring version - Degrees Degrees 152 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

151 3.3 Measure workpiece (milling) Parameters Description Unit _OVI [5] Probe number - _OVI [9] Alarm number - 1) For deactivated transformation, otherwise basic coordinate system Corner - any corner (CYCLE961) Function This measuring method can be used to measure the inside or outside corner of an unknown workpiece geometry. The measurements are performed paraxially to the active workpiece coordinate system. In addition to the measurement, the position of the corner can be used as workpiece zero in a specified work offset (WO). Measuring principle The measuring cycle traverses to the four measuring points (P1 to P4) one after the other and establishes the point of intersection of the resulting straight lines and the angle of rotation to the reference edge of measuring points P1 and P2 to the 1st axis of the plane (X for G17) in the positive direction The result (the position of the corner) is saved as an absolute value in the result parameters _OVR[ ] and optionally in the specified work offset (offset and rotation). The measured corner is shifted by the values in setpoint parameter (X0, Y0 for G17) in the workpiece coordinate system in the plane. The position of points P1 and P2 in relation to each other determines the direction of the 1st axis of the plane of the new coordinate system. Measure: Any corner, inside (CYCLE961) Measure: Any corner, outside (CYCLE961) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 153

152 3.3 Measure workpiece (milling) Requirements The probe must be called as a tool with a tool length compensation. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) Starting position before the measurement The probe is at the measuring height or above the corner (see protection zone) compared to the corner to be measured or in front of the 1st measuring point. The measuring points must be able to be approached from here collision-free. The measuring cycle generates the required traversing blocks and performs the measurements at the measuring points P1 to P4, starting with P1. Positioning measuring points P1 to P4 taking into account a protection zone Protection zone = no The probe is pre-positioned at the measuring height and remains at this measuring height when measuring the corner. An outer corner is traversed around. Protection zone = yes The probe is pre-positioned above the corner. When measuring, the 3rd axis of the plane (Z for G17) is moved by the value in parameter DZ to the measuring height, and the corresponding measuring point is measured. After the measurement, the probe is raised by the value of parameter DZ and moves to the next measuring point, where it is lowered again. Image 3-14 Protection zone = yes: Traversing around the outer corner with DZ>0 (measuring height + DZ) for G17 Position after the end of the measuring cycle After the last measurement, the probe is at measuring point P4. Depending on the protection zone parameter (yes/no), the probe is at the measuring height or above the corner. 154 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

153 3.3 Measure workpiece (milling) Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Corner" softkey. 3. Press the "Any corner" softkey. The input window "Measure: Any corner" opens Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit PL Measuring plane (G17 - G19) - T Name of the probe - Calibration data set (1-12) - D Cutting edge number (1-9) - Calibration data set (1-12) - X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured values in an adjustable WO) 1) - Coordinate system Polar Right-angled Position Type of corner: - Position of the corner Outside corner Inside corner - X0 Setpoint X of the measured corner (X for G17) mm Y0 Setpoint Y of the measured corner (X for G17) mm Only for coordinate system = "Polar": XP Position of the pole in the 1st axis of the plane (X for G17) mm YP Position of the pole in the 2nd axis of the plane (Y for G17) mm α0 Angle between X axis and the 1st edge (for G17) Degrees L1 Distance to the start position of the 1st measurement mm L2 Distance to the start position of the 2nd measurement mm α1 Opening angle Degrees - - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 155

154 3.3 Measure workpiece (milling) Parameter Description Unit L3 Distance to the start position of the 3rd measurement mm L4 Distance to the start position of the 4th measurement mm Only for coordinate system = "Right-angled": X1 Start position X of the 1st measurement mm Y1 Start position Y of the 1st measurement mm X2 Start position X of the 2nd measurement mm Y2 Start position Y of the 2nd measurement mm X3 Start position X of the 3rd measurement mm Y3 Start position Y of the 3rd measurement mm X4 Start position X of the 4th measurement mm Y4 Start position Y of the 4th measurement mm Protection zone Use protection zone - Yes No DZ Infeed distance at measuring height (only for protection zone "Yes") mm DFA Measurement path mm TSA Safe area for the measurement result mm 1) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. Machine manufacturer Please observe the machine manufacturer s instructions. Note The four measuring points or the measuring path DFA must be selected so that contour within the total path: 2 DFA [in mm] is reached. Otherwise, no measurement will be able to be made. Internally in the cycle, a minimum value of 20 mm for the measurement distance DFA is generated. 156 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

155 3.3 Measure workpiece (milling) Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Corner" softkey. 3. Press the "Any corner" softkey. The input window "Measure: Any corner" opens Parameter ShopTurn program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Calibration data set (1-12) - X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm List of the result parameters The measuring variant "Any corner" provides the following result parameters: Table 3-19 "Any corner" result parameters Parameters Description Unit _OVR [4] Angle actual value to the 1st axis of the plane in the workpiece coordinate system (WCS) _OVR [5] Corner point actual value in the 1st axis of the plane in the WCS mm _OVR [6] Corner point actual value in the 2nd axis of the plane in the WCS mm _OVR [20] Angle actual value to the 1st axis of plane in the machine coordinate system (MCS) 1) _OVR [21] Corner point actual value in the 1st axis of the plane in the MCS 1) mm _OVR [22] Corner point actual value in the 2nd axis of the plane in the MCS 1) mm _OVI [2] Measuring cycle number - _OVI [3] Measuring version - _OVI [5] Probe number - _OVI [9] Alarm number - 1) For deactivated transformation, otherwise basic coordinate system Degrees Degrees Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 157

156 3.3 Measure workpiece (milling) Hole - rectangular pocket (CYCLE977) Function This measuring method can be used to measure a rectangular pocket in a workpiece. The pocket width and the pocket length are measured and the pocket center point is determined. The measurements are always performed parallel to the geometry axis of the active plane. Measurements are also possible at a rectangular pocket rotated around the infeed axis. To do this, an angle corresponding to the real pocket position must be entered into the parameterization screen form. Probing at the sides of the pocket is always at right angles to these. A protection zone can be defined in the pocket. With the "3D probe with spindle reversal" measuring method, measurement is performed in the axes of the plane as differential measurement. Two complete measurements of the rectangular pocket are automatically carried out one after the other, one with a spindle position of 180 degrees, and one with 0 degrees. The special procedure for this measurement permits the use of an uncalibrated multi-directional probe. However, the correct tool radius of the probe must be determined once by calibrating the probe. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. With the "Align 3D probe" measuring method, the switching direction of the probe is always aligned to the current measuring direction. This function is recommended when high demands are placed on the measuring accuracy. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. The measurement result (measurement difference) can be used as follows: Correction of a WO so that the workpiece zero point is in relation to the center point of the rectangle Offset of a tool Measurement without offset 158 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

157 3.3 Measure workpiece (milling) Measuring principle Two opposite points in each of the two geometry axes of the plane are measured. The measurements start in the positive direction of the 1st geometry axis. From the four measured actual positions of the pocket sides, the pocket width and the pocket length are calculated, taking into account the calibration values. The position of the pocket center as workpiece zero is determined corresponding to the work offset selected to be corrected. The measuring differences of the side lengths are used as the basic quantity for a tool offset, the position of the pocket zero point as basis for the work offset. Measure: Rectangular pocket (CYCLE977) Measure: Rectangular pocket with protection zone (CYCLE977) Preconditions The probe must be active as tool. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) Star-type probe (type 714) Note The following measuring methods are only possible in the axes of the plane: 3D probe with spindle reversal (differential measurement) Align 3D probe The probe types 712, 713 and 714 generally cannot be used for these measuring methods. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 159

158 3.3 Measure workpiece (milling) Starting position before the measurement The probe must be positioned at the position setpoint of the pocket center point. This position approached in the pocket represents the starting position and at the same time the setpoint for the offsets to be determined. For a protection zone, the position of the probe ball is at a height above the protection zone. With the infeed path that has been entered, it must be guaranteed that from this height the desired measuring height in the pocket can be reached. Note If too large a measurement path DFA has been selected so that the protection zone is violated, then the distance is reduced automatically in the cycle. However, there must be sufficient room for the probe ball. Position after the end of the measuring cycle Without activated protection zone, at the end of the measuring cycle, the probe ball is at the measuring height in the center of the pocket. With a protection zone, at the end of the measuring cycle, the probe ball is centered above the pocket at the height of the starting position of the measuring cycles. Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Hole" softkey. 3. Press the "Rectangular pocket" softkey. The input window "Measure: Rectangular pocket" opens. 160 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

159 3.3 Measure workpiece (milling) Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) PL Measuring plane (G17 - G19) - Measuring method Calibration data set (1-12) (only for measuring without spindle reversal) - T Name of the probe - D Cutting edge number (1-9) - Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) - Calibration data set (1-12) (only for measuring without spindle reversal) X Y Z Start position X of the measurement Start position Y of the measurement Start position Z of the measurement - - mm mm mm Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured values in an adjustable WO) 3) Tool offset (save measured values in the tool data) TR Name of tool to be corrected - D Cutting edge number of tool to be corrected - W Pocket width setpoint mm L Pocket length setpoint mm α0 Angle between measuring axis and workpiece Degrees Protection zone Use protection zone Yes No WS Width of the protection zone (only for protection zone "Yes") mm LS Length of the protection zone (only for protection zone "Yes") mm DX / DY / DZ Infeed distance at measuring height (only for protection zone "Yes") mm DFA Measurement path mm TSA Safe area for the measurement result mm Dimensional tolerance Use dimensional tolerance for tool offset Yes No Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 161

160 3.3 Measure workpiece (milling) Parameter Description Unit TUL TLL Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") 1) The "3D probe with spindle reversal" function is shown if bit 16 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 2) The "Align 3D probe" function is shown if bit 17 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 3) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. mm mm Machine manufacturer Please observe the machine manufacturer s instructions. Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Hole" softkey. Parameter ShopTurn program 3. Press the "Rectangular pocket" softkey. The input window "Measure: Rectangular pocket" opens. Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) Calibration data set (1-12) (only for measuring without spindle reversal) X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

161 3.3 Measure workpiece (milling) List of the result parameters The measuring variant "Rectangular pocket" provides the following result parameters: Table 3-20 "Rectangular pocket" result parameters Parameters Description Unit _OVR [0] Rectangle length setpoint in the 1st axis of the plane mm _OVR [1] Rectangle length setpoint in the 2nd axis of the plane mm _OVR [2] Rectangle center point setpoint in the 1st axis of the plane mm _OVR [3] Rectangle center point setpoint in the 2nd axis of the plane mm _OVR [4] Rectangle length actual value in the 1st axis of the plane mm _OVR [5] Rectangle length actual value in the 2nd axis of the plane mm _OVR [6] Rectangle center point actual value in the 1st axis of the plane mm _OVR [7] Rectangle center point actual value in the 2nd axis of the plane mm _OVR [16] Rectangle length difference in the 1st axis of the plane mm _OVR [17] Rectangle length difference in the 2nd axis of the plane mm _OVR [18] Rectangle center point difference in the 1st axis of the plane mm _OVR [19] Rectangle center point difference in the 2nd axis of the plane mm _OVI [0] D number or WO number - _OVI [2] Measuring cycle number - _OVS_TNAME Tool name - For workpiece measurement with tool offset or correction in the work offset, additional parameters are displayed, seeadditional result parameters (Page 321) Hole - 1 hole (CYCLE977) Function This measuring method can be used to measure a hole in a workpiece. The hole diameter is measured as well as the hole center point determined. The measurements are always performed parallel to the geometry axis of the active plane. With a starting angle, the measuring points can be shifted to the periphery of the hole through rotation around the infeed axis as center point. A protection zone can be defined in the hole. With the "3D probe with spindle reversal" measuring method, measurement is performed in the axes of the plane as differential measurement. Two complete measurements of the bore are automatically carried out one after the other, one with a spindle position of 180 degrees, and one with 0 degrees. The special procedure for this measurement permits the use of an uncalibrated multi-directional probe. However, the correct tool radius of the probe must be determined once by calibrating the probe. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 163

162 3.3 Measure workpiece (milling) With the "Align 3D probe" measuring method, the switching direction of the probe is always aligned to the current measuring direction. This function is recommended when high demands are placed on the measuring accuracy. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. The measurement result (measurement difference) can be used as follows: Correction of a WO so that the workpiece zero point is in relation to the center of the hole Offset of a tool Measurement without offset Measuring principle Two opposite points in each of the two geometry axes of the plane are measured. The hole diameter and the center point are calculated from these four measured actual positions, taking into account the calibration values. From the measuring points of the 1st geometry axis of the plane, the center of this axis is calculated and the probe positioned at this center. Starting from this center point, the two points in the 2nd geometry axis are measured, from which the hole diameter is determined. The measurements start in the positive direction of the 1st geometry axis. The measured difference of the hole diameter is used for a tool offset and the position of the hole zero point as basis for a work offset. Measure: Hole (CYCLE977) Measure: Hole with protection zone (CY CLE977) Preconditions The probe must be active as tool. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) Star-type probe (type 714) 164 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

163 3.3 Measure workpiece (milling) Note The following measuring methods are only possible in the axes of the plane: 3D probe with spindle reversal (differential measurement) Align 3D probe The probe types 712, 713 and 714 generally cannot be used for these measuring methods. Starting position before the measurement The probe must be positioned at the position setpoint of the hole center point. This position approached in the hole represents the starting position and at the same time the setpoint for the offsets to be determined. For a protection zone, the center of the probe ball is at a height above the protection zone. With the infeed path that has been entered, it must be guaranteed that from this height the desired measuring height in the hole can be reached. Note If too large a measurement path DFA has been selected so that the protection zone is violated, then the distance is reduced automatically in the cycle. However, there must be sufficient room for the probe ball. Position after the end of the measuring cycle Without activated protection zone, the probe ball is at the measuring height in the center of the hole. With a protection zone, the measuring cycle end position of the probe ball is centered above the hole at the height of the starting position. Note The range of the measuring cycle starting points with regard to the hole center point must be within the value of the measuring path DFA, otherwise, there is danger of collision or the measurement cannot be performed! Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 165

164 3.3 Measure workpiece (milling) Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Hole" softkey. 3. Press the "1 hole" softkey. The input window "Measure: 1 hole" opens. Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) PL Measuring plane (G17 - G19) - Measuring method Calibration data set (1-12) (only for measuring without spindle reversal) - T Name of the probe - D Cutting edge number (1-9) - Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) - Calibration data set (1-12) (only for measuring without spindle reversal) X Y Z Start position X of the measurement Start position Y of the measurement Start position Z of the measurement - - mm mm mm Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured values in an adjustable WO) 3) Tool offset (save measured values in the tool data) TR Name of tool to be corrected - D Cutting edge number of tool to be corrected - Hole diameter setpoint mm α0 Angle between measuring axis and workpiece Degrees Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

165 3.3 Measure workpiece (milling) Parameter Description Unit Protection zone Use protection zone Yes No S Diameter of the protection zone (only for protection zone "Yes") mm LS Length of the protection zone (only for protection zone "Yes") mm DX / DY / DZ Infeed distance at measuring height (only for protection zone "Yes") mm DFA Measurement path mm TSA Safe area for the measurement result mm Dimensional tolerance TUL TLL Use dimensional tolerance for tool offset Yes No Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") 1) The "3D probe with spindle reversal" function is shown if bit 16 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 2) The "Align 3D probe" function is shown if bit 17 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 3) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. - - mm mm Machine manufacturer Please observe the machine manufacturer s instructions. Measuring version, milling on a lathe Procedure 1. Press the "Meas. workpiece" softkey. 2. Press the "Hole" softkey. 3. Press the "1 hole" softkey. The input window "Measure: 1 hole" opens. Parameter ShopTurn program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Measuring method Standard measuring method - 3D probe with spindle reversal 1) Align 3D probe 2) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 167

166 3.3 Measure workpiece (milling) ShopTurn program Parameter Description Unit Calibration data set (1-12) (only for measuring without spindle reversal) X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm - List of the result parameters The measuring variant "Hole" provides the following result parameters: Table 3-21 "Hole" result parameters Parameters Description Unit _OVR [0] Hole diameter setpoint mm _OVR [1] Hole center point setpoint in the 1st axis of the plane mm _OVR [2] Hole center point setpoint in the 2nd axis of the plane mm _OVR [4] Hole diameter actual value mm _OVR [5] Hole center point actual value in the 1st axis of the plane mm _OVR [6] Hole center point actual value in the 2nd axis of the plane mm _OVR [16] Hole diameter difference mm _OVR [17] Hole center point difference in the 1st axis of the plane mm _OVR [18] Hole center point difference in the 2nd axis of the plane mm _OVI [0] D number or WO number - _OVI [2] Measuring cycle number - _OVI [3] Measuring version - _OVS_TNAME Tool name - For workpiece measurement with tool offset or correction in the work offset, additional parameters are displayed, seeadditional result parameters (Page 321) Hole - inner circle segment (CYCLE979) Function This measuring version can be used to measure a circle segment from the inside. The diameter and the center point of the circle segment in the plane are determined. With a starting angle, referred to the 1st geometry axis of the plane, the measuring points can be shifted along the circumference of the circle segment. The distance between the measuring points along the circumference is defined using an incremental angle. With the "3D probe with spindle reversal" measuring method, measurement is performed in the axes of the plane as differential measurement. The special procedure for this measurement 168 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

167 3.3 Measure workpiece (milling) permits the use of an uncalibrated multidirectional probe. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. With the "Align 3D probe" measuring method, the switching direction of the probe is always aligned to the current measuring direction. This function is recommended when high demands are placed on the measuring accuracy. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. The measurement result (measurement difference) can be used as follows: Correction of a ZO so that the workpiece zero point is in relation to the circle segment center point. Offset of a tool Measurement without offset Measuring principle The circle segment can be measured with 3 or 4 measuring points. The intermediate positions to the measuring points are not approached along a circular path parallel to the geometry axis. The distance between the probe ball circumference and the hole corresponds to the measuring path DFA. The direction of the circular path is obtained from the sign of the incremental angle. The measuring path from the intermediate positions to the measuring points is radial to the hole periphery. The circle segment obtained from the number of measuring points and the incremental angle must not exceed 360 degrees. The measured difference of the segment diameter is used as tool offset, the segment zero as a basis for a zero offset. Image 3-15 Measure: Circle segment inner (CYCLE979), example 4 measuring points Requirements The probe must be active as tool. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 169

168 3.3 Measure workpiece (milling) Note The following measuring methods are only possible in the axes of the plane: 3D probe with spindle reversal (differential measurement) Align 3D probe The probe types 712, 713 and 714 generally cannot be used for these measuring methods. Note When measuring circle segments of < 90 degrees, it should be noted that, mathematically speaking, measuring points that deviate from the circular shape exert a particularly great influence on the accuracy of the results (center point, diameter). For this reason, an especially high degree of care should be taken when measuring small circle segments. Good results can be attained if the following procedures are used: The circle segment to be measured should be: Free from machining residue. Have as exact a circular form as possible, guaranteed by the machining technology. Have as smooth a surface as possible, guaranteed by the machining technology. Measured with high-quality probes, i.e. the shape of the probe ball is as homogeneous as possible. Measured with four points (setting via parameters). Measured with a recently calibrated probe. Starting position before the measurement The probe should be positioned in the 3rd axis of the plane (tool axis) at the required measuring height, approx. at a distance of the measuring path DFA in front of the first measuring point. Position after the end of the measuring cycle After measuring, the probe ball circumference is a distance of the measuring path DFA radially from the last measuring point at the measuring height. Note The range of the measuring cycle starting points with regard to the circle segment center point must be within the value of the measuring path DFA, otherwise, there is danger of collision or the measurement cannot be performed! 170 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

169 3.3 Measure workpiece (milling) Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Hole" softkey. 3. Press the "Inner circle segment" softkey. The input window "Measure: Inner circle segment" opens. Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) PL Measuring plane (G17 - G19) - Measuring method Calibration data set (1-12) (only for measuring without spindle reversal) - T Name of the probe - D Cutting edge number (1-9) - Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) - Calibration data set (1-12) (only for measuring without spindle reversal) X Y Z Start position X of the measurement Start position Y of the measurement Start position Z of the measurement - - mm mm mm Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured values in an adjustable WO) 3) Tool offset (save measured values in the tool data) TR Name of tool to be corrected - D Cutting edge number of tool to be corrected - Qty. measuring points Measurement with: 3 points 4 points Diameter of hole mm - - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 171

170 3.3 Measure workpiece (milling) Parameter Description Unit XM Center point X (for measuring plane G17) mm YM Center point Y (for measuring plane G17) mm α0 Starting angle Degrees α1 Incrementing angle Degrees DFA Measurement path mm TSA Safe area for the measurement result mm Dimensional tolerance TUL TLL Use dimensional tolerance for tool offset Yes No Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") 1) The "3D probe with spindle reversal" function is shown if bit 16 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 2) The "Align 3D probe" function is shown if bit 17 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 3) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. - mm mm Machine manufacturer Please observe the machine manufacturer s instructions. Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Hole" softkey. 3. Press the "Inner circle segment" softkey. The input window "Measure: Inner circle segment" opens. Parameter ShopTurn program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

171 3.3 Measure workpiece (milling) ShopTurn program Parameter Description Unit Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) Calibration data set (1-12) (only for measuring without spindle reversal) X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm - - List of the result parameters The measuring variant "Inner circle segment" provides the following result parameters: Table 3-22 "Inner circle segment" result parameters Parameters Description Unit _OVR [0] Hole diameter setpoint mm _OVR [1] Center point setpoint in the 1st axis of the plane mm _OVR [2] Center point setpoint in the 2nd axis of the plane mm _OVR [4] Hole diameter actual value mm _OVR [5] Center point actual value in the 1st axis of the plane mm _OVR [6] Center point actual value in the 2nd axis of the plane mm _OVR [16] Hole diameter difference mm _OVR [17] Center point difference in the 1st axis of the plane mm _OVR [18] Center point difference in the 2nd axis of the plane mm _OVI [0] D number or WO number - _OVI [2] Measuring cycle number - _OVI [3] Measuring version - _OVS_TNAME Tool name - For workpiece measurement with tool offset or correction in the work offset, additional parameters are displayed, seeadditional result parameters (Page 321) Spigot - rectangular spigot (CYCLE977) Function This measuring method can be used to measure a rectangular spigot on a workpiece. The spigot width and spigot length are measured as well as the spigot center point determined. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 173

172 3.3 Measure workpiece (milling) The measurements are always performed parallel to the geometry axis of the active plane. Measurements are also possible at a rectangular spigot rotated around the infeed axis. To do this, an angle corresponding to the real spigot position must be entered in the parameterization axis. Probing at the sides of the spigot is always at right angles to these. A protective zone can be defined around the spigot. With the "3D probe with spindle reversal" measuring method, measurement is performed in the axes of the plane as differential measurement. Two complete measurements of the rectangular spigot are automatically carried out one after the other, one with a spindle position of 180 degrees, and one with 0 degrees. The special procedure for this measurement permits the use of an uncalibrated multi-directional probe. However, the correct tool radius of the probe must be determined once by calibrating the probe. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. With the "Align 3D probe" measuring method, the switching direction of the probe is always aligned to the current measuring direction. This function is recommended when high demands are placed on the measuring accuracy. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. The measurement result (measurement difference) can be used as follows: Correction of a WO so that the workpiece zero point is in relation to the center point of the rectangular spigot Offset of a tool Measurement without offset Measuring principle Two opposite points in each of the two geometry axes of the plane are measured. The measurements start in the positive direction of the 1st geometry axis. The spigot width and the spigot length are calculated from the four measured actual positions of the spigot sides, taking into account the calibration values. Corresponding to the work offset selected to be corrected, the position of the spigot center is determined as the workpiece zero. The measuring differences of the side lengths are used as the basic quantity for a tool offset, the position of the spigot zero point as basis for the work offset. Measure: Rectangular spigot (CYCLE977) Measure: Rectangular spigot with protection zone (CYCLE977) 174 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

173 3.3 Measure workpiece (milling) Preconditions The probe must be active as tool. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) Star-type probe (type 714) Note The following measuring methods are only possible in the axes of the plane: 3D probe with spindle reversal (differential measurement) Align 3D probe The probe types 712, 713 and 714 generally cannot be used for these measuring methods. Starting position before the measurement The probe must be positioned above the rectangular spigot at the position setpoint of the center point. This position approached above the spigot represents the starting position and at the same time the setpoint for the offsets to be determined. With the infeed path that has been entered, it must be guaranteed that from the starting position height, the desired measuring height at the rectangular spigot can be reached. A protection zone has no effect on the starting position. Note If too large a measurement path DFA has been selected so that the protection zone is violated, then the distance is reduced automatically in the cycle. However, there must be sufficient room for the probe ball. Position after the end of the measuring cycle The measuring cycle end position of the probe ball is centered above the spigot at the height of the measuring cycles starting position. Note The range of the cycle starting positions with regard to the spigot center point must be within the value of the measuring path DFA, otherwise, there is danger of collision or the measurement cannot be performed! Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 175

174 3.3 Measure workpiece (milling) Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Spigot" softkey. 3. Press the "Rectangular spigot" softkey. The input window "Measure: Rectangular spigot" opens. Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) PL Measuring plane (G17 - G19) - Measuring method Calibration data set (1-12) (only for measuring without spindle reversal) - T Name of the probe - D Cutting edge number (1-9) - Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) - Calibration data set (1-12) (only for measuring without spindle reversal) X Y Z Start position X of the measurement Start position Y of the measurement Start position Z of the measurement - - mm mm mm Parameter Description Unit Correction target Measuring only (no offset) - Work offset (save measured values in an adjustable WO) 3) Tool offset (save measured values in the tool data) TR Name of tool to be corrected - D Cutting edge number of tool to be corrected - W Setpoint, spigot width mm L Setpoint, spigot length mm α0 Angle between measuring axis and workpiece Degrees 176 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

175 3.3 Measure workpiece (milling) Parameter Description Unit DZ Infeed distance at measuring height (for G17) mm Protection zone Use protection zone Yes No WS Width of the protection zone (only for protection zone "Yes") mm LS Length of the protection zone (only for protection zone "Yes") mm DFA Measurement path mm TSA Safe area for the measurement result mm Dimensional tolerance TUL TLL Use dimensional tolerance for tool offset Yes No Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") 1) The "3D probe with spindle reversal" function is shown if bit 16 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 2) The "Align 3D probe" function is shown if bit 17 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 3) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. - - mm mm Machine manufacturer Please observe the machine manufacturer s instructions. Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Spigot" softkey. 3. Press the "Rectangular spigot" softkey. The input window "Measure: Rectangular spigot" opens. Parameter ShopTurn program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 177

176 3.3 Measure workpiece (milling) ShopTurn program Parameter Description Unit Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) Calibration data set (1-12) (only for measuring without spindle reversal) X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm - - List of the result parameters The measuring variant "Rectangular spigot" provides the following result parameters: Table 3-23 "Rectangular spigot" result parameters Parameters Description Unit _OVR [0] Rectangle length setpoint in the 1st axis of the plane mm _OVR [1] Rectangle length setpoint in the 2nd axis of the plane mm _OVR [2] Rectangle center point setpoint in the 1st axis of the plane mm _OVR [3] Rectangle center point setpoint in the 2nd axis of the plane mm _OVR [4] Rectangle length actual value in the 1st axis of the plane mm _OVR [5] Rectangle length actual value in the 2nd axis of the plane mm _OVR [6] Rectangle center point actual value in the 1st axis of the plane mm _OVR [7] Rectangle center point actual value in the 2nd axis of the plane mm _OVR [16] Rectangle length difference in the 1st axis of the plane mm _OVR [17] Rectangle length difference in the 2nd axis of the plane mm _OVR [18] Rectangle center point difference in the 1st axis of the plane mm _OVR [19] Rectangle center point difference in the 2nd axis of the plane mm _OVI [0] D number or WO number - _OVI [2] Measuring cycle number - _OVI [3] Measuring version - _OVS_TNAME Tool name - For workpiece measurement with tool offset or correction in the work offset, additional parameters are displayed, seeadditional result parameters (Page 321). 178 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

177 3.3 Measure workpiece (milling) Spigot - 1 circular spigot (CYCLE977) Function This measuring method can be used to measure a circular spigot on a workpiece. The spigot diameter is measured and the spigot center point is determined. The measurements are always performed parallel to the geometry axis of the active plane. With a starting angle, the measuring points can be shifted along the circumference of the spigot around the infeed axis as center of rotation. A protective zone can be defined around the spigot. With the "3D probe with spindle reversal" measuring method, measurement is performed in the axes of the plane as differential measurement. Two complete measurements of the spigot are automatically carried out one after the other, one with a spindle position of 180 degrees, and one with 0 degrees. The special procedure for this measurement permits the use of an uncalibrated multi-directional probe. However, the correct tool radius of the probe must be determined once by calibrating the probe. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. With the "Align 3D probe" measuring method, the switching direction of the probe is always aligned to the current measuring direction. This function is recommended when high demands are placed on the measuring accuracy. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. The measurement result (measurement difference) can be used as follows: Correction of a WO so that the zero point is in relation to the center point of the spigot Offset of a tool Measurement without offset Measuring principle Two opposite points in each of the two geometry axes of the plane are measured. The spigot diameter and the center point are calculated from these four measured actual positions, taking into account the calibration values. From the measuring points of the 1st geometry axis of the plane, the center of this axis is calculated and the probe positioned at this center. Starting from this center point, the two points in the 2nd geometry axis are measured, from which the actual spigot diameter is determined. The measurements start in the positive Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 179

178 3.3 Measure workpiece (milling) direction of the 1st geometry axis. The measured difference of the spigot diameter is used as tool offset and the position of the spigot zero point as basis for a work offset. Measure: Circular spigot (CYCLE977) Measure: Circular spigot with protection zone (CYCLE977) Preconditions The probe must be active as tool. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) Star-type probe (type 714) Note The following measuring methods are only possible in the axes of the plane: 3D probe with spindle reversal (differential measurement) Align 3D probe The probe types 712, 713 and 714 generally cannot be used for these measuring methods. Starting position before the measurement The probe must be positioned above the circular spigot at the position setpoint of the center point. This position approached above the spigot represents the starting position and at the same time the setpoint for the offsets to be determined. With the infeed path that has been entered, it must be guaranteed that from the starting position height, the desired measuring height at the spigot can be reached. 180 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

179 3.3 Measure workpiece (milling) A protection zone has no effect on the starting position. Note If too large a measurement path DFA has been selected so that the protection zone is violated, then the distance is reduced automatically in the cycle. However, there must be sufficient room for the probe ball. Position after the end of the measuring cycle The measuring cycle end position of the probe ball is centered above the spigot at the height of the measuring cycles starting position. Note The range of the measuring cycle starting positions with regard to the spigot center point must be within the value of the measuring path DFA, otherwise, there is danger of collision or the measurement cannot be performed! Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Spigot" softkey. 3. Press the "1 circular spigot" softkey. The input window "Measure: 1 circular spigot" opens. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 181

180 3.3 Measure workpiece (milling) Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) PL Measuring plane (G17 - G19) - Measuring method Calibration data set (1-12) (only for measuring without spindle reversal) - T Name of the probe - D Cutting edge number (1-9) - Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) - Calibration data set (1-12) (only for measuring without spindle reversal) X Y Z Start position X of the measurement Start position Y of the measurement Start position Z of the measurement - - mm mm mm Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured values in an adjustable WO) 3) Tool offset (save measured values in the tool data) TR Name of tool to be corrected - D Cutting edge number of tool to be corrected - Spigot diameter setpoint mm α0 Angle between measuring axis and workpiece Degrees DZ Infeed distance at measuring height (for G17) mm Protection zone Use protection zone Yes No S Diameter of the protection zone (only for protection zone "Yes") mm DFA Measurement path mm TSA Safe area for the measurement result mm Dimensional tolerance Use dimensional tolerance for tool offset Yes No Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

181 3.3 Measure workpiece (milling) Parameter Description Unit TUL TLL Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") 1) The "3D probe with spindle reversal" function is shown if bit 16 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 2) The "Align 3D probe" function is shown if bit 17 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 3) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. mm mm Machine manufacturer Please observe the machine manufacturer s instructions. Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Spigot" softkey. Parameter ShopTurn program 3. Press the "1 circular spigot" softkey. The input window "Measure: 1 circular spigot" opens. Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) Calibration data set (1-12) (only for measuring without spindle reversal) X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm - - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 183

182 3.3 Measure workpiece (milling) List of the result parameters The measuring variant "1 circular spigot" provides the following result parameters: Table 3-24 "1 circular spigot" result parameters Parameters Description Unit _OVR [0] Circular spigot diameter setpoint mm _OVR [1] Circular spigot center point setpoint in the 1st axis of the plane mm _OVR [2] Circular spigot center point setpoint in the 2nd axis of the plane mm _OVR [4] Circular spigot diameter actual value mm _OVR [5] Circular spigot center point actual value in the 1st axis of the plane mm _OVR [6] Circular spigot center point actual value in the 2nd axis of the plane mm _OVR [16] Circular spigot diameter difference mm _OVR [17] Circular spigot center point difference in the 1st axis of the plane mm _OVR [18] Circular spigot center point difference in the 2nd axis of the plane mm _OVI [0] D number or WO number - _OVI [2] Measuring cycle number - _OVI [3] Measuring version - _OVS_TNAME Tool name - For workpiece measurement with tool offset or correction in the work offset, additional parameters are displayed, seeadditional result parameters (Page 321) Spigot - outer circle segment (CYCLE979) Function This measuring version can be used to measure circle segment from the outside. The diameter and the center point of the circle segment in the plane are determined. With a starting angle, referred to the 1st geometry axis of the plane, the measuring points can be shifted along the circumference of the circle segment. The distance between the measuring points along the circumference is defined using an incremental angle. With the "3D probe with spindle reversal" measuring method, measurement is performed in the axes of the plane as differential measurement. The special procedure for this measurement permits the use of an uncalibrated multidirectional probe. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. With the "Align 3D probe" measuring method, the switching direction of the probe is always aligned to the current measuring direction. This function is recommended when high demands are placed on the measuring accuracy. Probe types 712, 713 and 714 are not suitable for this purpose. A positionable spindle is mandatory. 184 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

183 3.3 Measure workpiece (milling) The measurement result (measurement difference) can be used as follows: Correction of a ZO so that the workpiece zero point is in relation to the circle segment center point. Offset of a tool Measurement without offset Measuring principle The circle segment can be measured with three or four measuring points. The intermediate positions to the measuring points are not approached along a circular path parallel to the geometry axis. The distance between the probe ball circumference and the hole corresponds to the measuring path DFA. The direction of the circular path is obtained from the sign of the incremental angle. The measuring path from the intermediate positions to the measuring points is radial to the hole periphery. The circle segment obtained from the number of measuring points and the incremental angle must not exceed 360 degrees. The measured difference of the segment diameter is used as tool offset, the segment zero point as a basis for a zero offset. Image 3-16 Measure: Outer circle segment (CYCLE977) Requirements The probe must be active as tool. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 185

184 3.3 Measure workpiece (milling) Note The following measuring methods are only possible in the axes of the plane: 3D probe with spindle reversal (differential measurement) Align 3D probe The probe types 712, 713 and 714 generally cannot be used for these measuring methods. Note When measuring circle segments of < 90 degrees, it should be noted that, mathematically speaking, measuring points that deviate from the circular shape exert a particularly great influence on the accuracy of the results (center point, diameter). For this reason, an especially high degree of care should be taken when measuring small circle segments. Good results can be attained if the following procedures are used: The circle segment to be measured should be: Free from machining residue. Have as exact a circular form as possible, guaranteed by the machining technology. Have as smooth a surface as possible, guaranteed by the machining technology. Measured with high-quality probes, i.e. the shape of the probe ball is as homogeneous as possible. Measured with four points (setting via parameters). Measured with a recently calibrated probe. Starting position before the measurement The probe should be positioned in the 3rd axis of the plane (tool axis) at the required measuring height, approx. at a distance of the measuring path DFA in front of the first measuring point. Position after the end of the measuring cycle At the end of the measurement, the probe ball circumference is a distance of the measuring path DFA radially from the last measuring point at the measuring height. Note The range of the measuring cycle starting points with regard to the circle segment center point must be within the value of the measuring path DFA, otherwise, there is danger of collision or the measurement cannot be performed! 186 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

185 3.3 Measure workpiece (milling) Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Spigot" softkey. 3. Press the "Outer circle segment" softkey. The input window "Measure: Outer circle segment" opens. Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) PL Measuring plane (G17 - G19) - Measuring method Calibration data set (1-12) (only for measuring without spindle reversal) - T Name of the probe - D Cutting edge number (1-9) - Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) - Calibration data set (1-12) (only for measuring without spindle reversal) X Y Z Start position X of the measurement Start position Y of the measurement Start position Z of the measurement - - mm mm mm Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured values in an adjustable WO) 3) Tool offset (save measured values in the tool data) TR Name of tool to be corrected - D Cutting edge number of tool to be corrected - Qty. measuring points Measurement with: 3 points 4 points - - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 187

186 3.3 Measure workpiece (milling) Parameter Description Unit Diameter of spigot mm XM Center point X (for measuring plane G17) mm YM Center point Y (for measuring plane G17) mm α0 Starting angle Degrees α1 Incrementing angle Degrees DFA Measurement path mm TSA Safe area for the measurement result mm Dimensional tolerance TUL TLL Use dimensional tolerance for tool offset Yes No Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") 1) The "3D probe with spindle reversal" function is shown if bit 16 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 2) The "Align 3D probe" function is shown if bit 17 is set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. 3) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. - mm mm Machine manufacturer Please observe the machine manufacturer s instructions. Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "Spigot" softkey. 3. Press the "Outer circle segment" softkey. The input window "Measure: Outer circle segment" opens. Parameter ShopTurn program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

187 3.3 Measure workpiece (milling) ShopTurn program Parameter Description Unit Measuring method Standard measuring method 3D probe with spindle reversal 1) Align 3D probe 2) Calibration data set (1-12) (only for measuring without spindle reversal) X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm - - List of the result parameters The measuring variant "Outer circle segment" provides the following result parameters: Table 3-25 "Outer circle segment" result parameters Parameters Description Unit _OVR [0] Circle segment diameter setpoint mm _OVR [1] Center point setpoint in the 1st axis of the plane mm _OVR [2] Center point setpoint in the 2nd axis of the plane mm _OVR [4] Circle segment diameter actual value mm _OVR [5] Center point actual value in the 1st axis of the plane mm _OVR [6] Center point actual value in the 2nd axis of the plane mm _OVR [16] Circle segment diameter difference mm _OVR [17] Center point difference in the 1st axis of the plane mm _OVR [18] Center point difference in the 2nd axis of the plane mm _OVI [0] D number or WO number - _OVI [2] Measuring cycle number - _OVI [3] Measuring version - _OVS_TNAME Tool name - For workpiece measurement with tool offset or correction in the work offset, additional parameters are displayed, seeadditional result parameters (Page 321) D - align plane (CYCLE998) Function This measuring variant can be used to determine and correct the angular position of a threedimensional inclined plane on a workpiece by measuring three points. The angles are in relation to the rotation around the axes of the active plane G17 to G19. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 189

188 3.3 Measure workpiece (milling) The same requirements as for the simple angle measurement apply, see measuring version Align edge (Page 131). Additional data are required for the setpoint input of the 2nd angle. A correction is made in the zero offset in the rotary components (rotation) of the specified zero offset (ZO). The translatory components of the ZO remain unchanged, and should be corrected in a subsequent measurement (e.g. set edge, corner). After the measurement, at suitable machines where orientation transformation (swiveling, TRAORI) is set up, the probe can be aligned perpendicular on the measuring plane (machining plane). Swiveling: See the Programming Manual SINUMERIK 840D sl/840d/840di sl cycles, Chapter "Swiveling - CYCLE800". TRAORI G0 C3=1 ;align to tool axis Z for G17 Measuring principle The "Align plane" measuring variant is performed according to the 2-angle measurement principle: The angular offsets are in the rotary part of the geometry axes for a workpiece with a threedimensional inclined plane. Image 3-17 Measure: Align plane (CYCLE998) Note Maximum measured angle The CYCLE998 measuring cycle is capable of measuring a maximum angle of degrees. 190 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

189 3.3 Measure workpiece (milling) Requirements The probe must be called as a tool with a tool length compensation. Tool type of the probe: 3D multi probe (type 710) Mono probe (type 712) Starting position before the measurement The probe is pre-positioned over the 1st measuring point P1 in the axes of the plane (for G17: XY). Positioning taking into account a protection zone Protection zone "no" The probe is positioned in the measuring axis as a maximum at the distance of measurement path DFA above the surface to be measured above measuring point P1 at the measuring height. Protection zone "yes" The measuring probe is positioned in the measuring axis as a maximum at the distance of measurement path DFA and the amount in parameter DZ (for G17 always measuring axis Z) above the surface to be measured above measuring point P1 at the measuring height. In both cases, when making the measurement, measuring point P1 must be able to be safely reached. For the 1st measurement, if the distances from the reference surface are selected to be too large, then a measurement is not made. Measuring axis is always the 3rd axis of the plane (for G17: Z). Measuring point P1 should be selected in the plane so that the distance to the 2nd measuring point (L2) and to the 3rd measuring point (L3) results in positive values. Positioning between measuring points P1, P2, P3 Intermediate positioning "parallel to the plane" The probe traverses parallel to the reference surface at the distance of parameter L2 to measuring point P2, or after the 2nd measurement at the distance of parameter L3, to measuring point P3. In so doing, the angle from parameters α and TSA is taken into account. TSA contains the value for the maximum permissible angular deviation. After performing the measurement in P1, the probe is positioned to P2 in the 1st axis of the plane and in the 3rd axis of the plane (for G17 in X and Z) taking into account the angle β and a maximum deviation in TSA. After the measurement in P2 has been performed the probe is repositioned to P1 along the same path. The probe is positioned from P1 to P3 in the 2nd axis of the plane (for G17 in X and Y) and the 3rd axis of the plane taking into account angle α and maximum deviation in TSA and then a measurement performed. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 191

190 3.3 Measure workpiece (milling) Intermediate positioning "parallel to the axis" Positioning from P1 to P2 is performed in the 1st axis of the plane, from P1 to P3 in the 2nd axis of the plane. With the starting position P1 in the 3rd axis of the plane (for G17 in Z), P2 and/or P3 must also be able to be reached without any collision. Position after the end of the measuring cycle The probe is at a distance of the measurement path above the last measuring point (P3). Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "3D" softkey. 3. Press the "Align plane" softkey. The input window "Measure: Align plane" opens. Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit PL Measuring plane (G17 - G19) - T Name of the probe - Calibration data set (1-12) - D Cutting edge number (1-9) - X Y Z Calibration data set (1-12) - Start position X of the measurement Start position Y of the measurement Start position Z of the measurement mm mm mm Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured values in an adjustable WO) 1) - Positioning Position probe: Parallel to the axis Parallel to the plane α Inclination of the plane to the X axis (X for G17) Degrees L2X Distance to the 2nd measuring point in the direction of the X axis mm β Inclination of the plane to the Y axis (Y for G17) Degrees Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

191 3.3 Measure workpiece (milling) Parameter Description Unit L3X Distance to the 3rd measuring point in the direction of the X axis mm L3Y Distance to the 3rd measuring point in the direction of the Y axis mm Protection zone DZ (only for protection zone "Yes") Use protection zone Yes No Infeed path at the measuring height in the Z axis (for G17) DFA Measurement path mm TSA Safe area for the measurement result mm 1) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. - mm Machine manufacturer Please observe the machine manufacturer s instructions. Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "3D" softkey. 3. Press the "Align plane" softkey. The input window "Measure: Align plane" opens. Parameter ShopTurn program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Calibration data set (1-12) - X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 193

192 3.3 Measure workpiece (milling) List of the result parameters The measuring variant "Align plane" provides the following result parameters: Table 3-26 "Align plane" result parameters Parameters Description Unit _OVR [0] _OVR [1] _OVR [4] _OVR [5] Angle setpoint between workpiece surface and 1st axis of the plane of the active WCS Angle setpoint between workpiece surface and 2nd axis of the plane of the active WCS Angle actual value between workpiece surface and 1st axis of the plane of the active WCS Angle actual value between workpiece surface and 2nd axis of the plane of the active WCS Degrees Degrees Degrees Degrees _OVR [16] Angle difference around the 1st axis of the plane Degrees _OVR [17] Angle difference around the 2nd axis of the plane Degrees _OVR [20] Angle offset value Degrees _OVR [21] Angle offset value around the 1st axis of the plane Degrees _OVR [22] Angle offset value around the 2nd axis of the plane Degrees _OVR [23] Angle offset value around the 3rd axis of the plane Degrees _OVR [28] Safe area Degrees _OVR [30] Empirical value Degrees _OVI [0] WO number - _OVI [2] Measuring cycle number - _OVI [5] Probe number - _OVI [7] Empirical value memory number - _OVI [9] Alarm number - _OVI [11] Status offset request D - sphere (CYCLE997) Function This measuring variant can be used to measure a sphere. Measuring can be parallel to the axis or on a circular path in the workpiece coordinate system. The center point (position of the sphere) for a known diameter is determined from three or four measuring points at the circumference and one measuring point at the "north pole" of the sphere. With the selection "determine sphere diameter" and "no repeat measurement", using an additional measurement, the sphere diameter is correctly determined. For the selection "Determine sphere diameter" and "With repeat measurement", the additional measurement is carried out in the 1st pass only. 194 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

193 3.3 Measure workpiece (milling) In the 2nd pass (repeat pass), the diameter is internally calculated without an additional measurement. Measuring cycle CYCLE997 can measure the sphere and, in addition, automatically correct a work offset (WO) in the translational offsets of the three axes of the active plane on the basis of the position of the sphere center. Measuring principle The following description refers to the machining plane G17: Axes of the plane: XY Tool axis: Z Beginning at the starting position, the setpoint of the sphere equator is approached initially in -X and then in -Z. Three or four points are measured at this measuring height. Measure: Sphere (CYCLE997), Example of "paraxial" positioning Measure: Sphere (CYCLE997), Example of positioning "on a circular path" Measuring version "Paraxial positioning": When positioning between measuring points (e.g. P1-> P2, P2->P3), the axis always retracts to the starting position (at the north pole of the sphere). The angular position when measuring measuring point P1 is defined using the probe angle α0 (starting angle) Measuring version "Positioning on a circular path": Positioning between measuring points (e.g. P1-> P2, P2->P3) is realized on a circular path at the same height as the equator of the sphere. With probe angle α0 (starting angle), the angular position when the measuring point P1 is defined; with α1 the incremental angle to P2 and further to P3 and for the measuring version with four measuring points, to P4. The number of measuring points multiplied with the stepping angle α1 must not exceed 360 degrees. Internally, the actual center point of circle XY is determined from these measured values (sphere center in the plane). Then with +Z and in XY, the axis traverses to the calculated "north pole" of the sphere. A measurement is made there in -Z. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 195

194 3.3 Measure workpiece (milling) The complete center point of the sphere is calculated in the three axes of the plane (XYZ) from the measuring points. In the case of a repeat measurement, the axis traverses to the precise equator of the sphere (from the 1st measurement); this improves the measurement result. If, in addition to the sphere center point, also the actual sphere diameter is to be measured, then in the 1st measuring pass the cycle performs a supplementary measurement parallel to the axis at the equator in the +X direction. If "Repeat measurement" is selected, in the 2nd pass (repeat pass), then an additional measurement is not performed, and the diameter is internally calculated. The "Positioning on a circular path" measuring version should be preferably used, because this permits optimum positioning behavior. In addition, with this measuring version, when circling around the sphere, the probe can be aligned in the switching direction (see the "align probe" parameter). Correction in a work offset (WO) The set-actual differences of the center point coordinates are calculated in the translatory part of the WO. During the correction, the determined sphere center point includes the specified setpoint position (workpiece coordinates, three axes) in the corrected WO. Preconditions The probe must be called as a tool with tool length compensation and be active. Tool type of the probe: 3D multi probe (type 710) The sphere diameter must be significantly greater than the sphere diameter of the probe stylus. Starting position before the measurement The probe must be positioned above the set sphere center point at a safe height. The measuring cycle generates the traversing motion for approaching the measuring points itself and performs the measurements depending on the measuring version selected. Note The sphere to be measured must be mounted in such a way that when positioning the probe, the equator of the probe sphere of the measuring object can be reliably reached in the workpiece coordinate system and no collision with the sphere clamping occurs. By specifying a variable starting and incremental angle, when positioning on a circular path, this is also possible under difficult clamping conditions. The measurement path in parameter DFA should be selected so large that all measuring points can be reached within total measurement path 2 DFA. Otherwise no measurement can be performed or the measurements are incomplete. 196 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

195 3.3 Measure workpiece (milling) Position after the end of the measuring cycle The probe is above the determined sphere center point at a safe height (height at the starting position). Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "3D" softkey. 3. Press the "Sphere" softkey. The input window "Measure: Sphere" opens. Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit PL Measuring plane (G17 - G19) - T Name of the probe - Calibration data set (1-12) - D Cutting edge number (1-9) - X Y Z Calibration data set (1-12) - Start position X of the measurement Start position Y of the measurement Start position Z of the measurement mm mm mm Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured values in an adjustable WO) 1) - Positioning Traverse around sphere: Parallel to the axis On circular path Only for positioning "On circular path": Align probe Number of measuring points Always align probe in the same contact direction No Yes Measuring the sphere with three or four measuring points at the sphere equator Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 197

196 3.3 Measure workpiece (milling) Parameter Description Unit Repeat measurement Determining the sphere diameter Repeat measurement with determined values No Yes No Yes Sphere diameter setpoint mm α0 Contact angle (only for positioning "On circular path") Degrees α1 Incremental angle (only for positioning "On circular path") Degrees XM Center point of the sphere on the X axis (for G17) mm YM Center point of the sphere on the Y axis mm ZM Center point of the sphere on the Z axis mm DFA Measurement path mm TSA Safe area for the measurement result mm 1) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE. - - Machine manufacturer Please observe the machine manufacturer s instructions. Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "3D" softkey. 3. Press the "Sphere" softkey. The input window "Measure: Sphere" opens. Parameter ShopTurn program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Calibration data set (1-12) - X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm 198 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

197 3.3 Measure workpiece (milling) List of the result parameters The measuring variant "Sphere" provides the following result parameters: Table 3-27 "Sphere" result parameters Parameters Description Unit _OVR[0] Sphere diameter setpoint mm _OVR[1] Center point coordinate setpoint in the 1st axis of the plane mm _OVR[2] Center point coordinate setpoint in the 2nd axis of the plane mm _OVR[3] Center point coordinate setpoint in the 3rd axis of the plane mm _OVR[4] Sphere diameter actual value mm _OVR[5] Center point coordinate actual value in the 1st axis of the plane mm _OVR[6] Center point coordinate actual value in the 2nd axis of the plane mm _OVR[7] Center point coordinate actual value in the 3rd axis of the plane mm _OVR[8] Sphere diameter difference mm _OVR[9] Center point coordinate difference in the 1st axis of the plane mm _OVR[10] Center point coordinate difference in the 2nd axis of the plane mm _OVR[11] Center point coordinate difference in the 3rd axis of the plane mm _OVR[28] Safe area mm _OVI[0] WO number - _OVI[2] Measuring cycle number - _OVI[5] Probe number - _OVI[9] Alarm number - _OVI[11] Status offset request - _OVI[12] Supplementary error data for alarm, internal measurement evaluation D - 3 spheres (CYCLE997) Function This measuring method can be used to measure three balls of equal size, fixed to a common base (workpiece). Measuring individual balls is realized the same as when measuring one ball, see 3D ball (CYCLE997) (Page 194). After measuring the 3rd ball, for a correction in a work offset (WO), the position of the workpiece on which the balls are mounted, is corrected as a rotation in the WO. Measuring principle The position of the center points of the three balls should be entered as a setpoint in parameters XM1 to ZM3 in the active workpiece coordinate system. The measurement begins with the 1st ball and ends with the 3rd ball. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 199

198 3.3 Measure workpiece (milling) Positioning between the balls is realized along a straight line at the height of the starting position of the 1st ball. The parameter settings such as the number of measuring points, determining the diameter, diameter apply to all three balls. Measure: 3 balls (CYCLE997), Example of "paraxial positioning" Measure: 3 balls (CYCLE997), Example of "positioning on a circular path" Correcting the work offset (WO) After the measurement of the 3rd ball, a work offset is calculated from the measured center points of the balls. This consists of translatory components (offset) and rotary components (rotation), and describes the position of the workpiece on which the balls are mounted. During the correction, the triangle of the determined ball center points includes the specified center point setpoint position (workpiece coordinates). The sum of the deviations of the spheres to each other must be within the value of parameter TVL. Otherwise no correction is performed and an alarm is output. Requirements The probe must be called as a tool with tool length compensation and be active. Tool type of the probe: 3D multi probe (type 710) In the active WO, the approximate values for the position of the balls regarding offset and rotation are entered and activated. The value in the offset of the WO refers to the 1st ball. Only minor deviations from the actual position of workpiece from the cycle can be expected. The ball diameter must be significantly greater than the ball diameter of the probe stylus. 200 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

199 3.3 Measure workpiece (milling) Starting position before the measurement The probe must be positioned above the setpoint ball center point of the 1st ball at a safe height. Note The measuring points must be selected so that there is no danger of a collision with a ball fixture or another obstacle during measuring or intermediate positioning. The measurement path in parameter DFA should be selected so large that all measuring points can be reached within total measurement path 2 x DFA. Otherwise no measurement can be performed or the measurements are incomplete. Position after the end of the measuring cycle The probe is above the determined ball center point of the 3rd ball at a safe height (height at the starting position). Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "3D" softkey. 3. Press the "3 spheres" softkey. The input window "Measure: 3 spheres" opens. Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit PL Measuring plane (G17 - G19) - T Name of the probe - Calibration data set (1-12) - D Cutting edge number (1-9) - X Y Z Calibration data set (1-12) - Start position X of the measurement Start position Y of the measurement Start position Z of the measurement mm mm mm Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 201

200 3.3 Measure workpiece (milling) Parameter Description Unit Correction target Measuring only (no offset) Work offset (save measured values in an adjustable WO) 1) - Positioning Traverse around sphere: Parallel to the axis On circular path Only for positioning "On circular path": Align probe Number of measuring points Repeat measurement Determining the sphere diameter Always align probe in the same contact direction Yes No Measuring the spheres with three or four measuring points at the equator of the spheres - Repeat measurement with determined values Yes No Yes No Sphere diameter setpoint mm α0 Contact angle (only for positioning "On circular path") Degrees α1 Incremental angle (only for positioning "On circular path") Degrees XM1 Center point of the 1st sphere X axis mm YM1 Center point of the 1st sphere Y axis mm ZM1 Center point of the 1st sphere Z axis mm XM2 Center point of the 2nd sphere X axis mm YM2 Center point of the 2nd sphere Y axis mm ZM2 Center point of the 2nd sphere Z axis mm XM3 Center point of the 3rd sphere X axis mm YM3 Center point of the 3rd sphere Y axis mm ZM3 Center point of the 3rd sphere Z axis mm TVL Limit value of the minimum inside angle of the measured triangle of the three measurements of the rotary axes. DFA Measurement path mm TSA Safe area for the measurement result mm 1) Other parameters and correction targets can be set in the general SD $SNS_MEA_FUNCTION_MASK_PIECE Machine manufacturer Please observe the machine manufacturer s instructions. 202 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

201 3.3 Measure workpiece (milling) Measuring version, milling on a lathe Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "3D" softkey. 3. Press the "3 spheres" softkey. The input window "Measure: 3 spheres" opens. Parameter ShopTurn program Parameter Description Unit T Name of the probe - D Cutting edge number (1-9) - Calibration data set (1-12) - X Start position X of the measurement mm Y Start position Y of the measurement mm Z Start position Z of the measurement mm List of the result parameters The measuring variant "3 spheres" provides the following result parameters: Table 3-28 "3 spheres" result parameters Parameters Description Unit _OVR[0] Sphere diameter setpoint of 1st sphere mm _OVR[1] _OVR[2] _OVR[3] Center point coordinate setpoint in the 1st axis of the plane of the 1st sphere Center point coordinate setpoint in the 2nd axis of the plane of the 1st sphere Center point coordinate setpoint in the 3rd axis of the plane of the 1st sphere _OVR[4] Sphere diameter actual value of 1st sphere mm _OVR[5] _OVR[6] _OVR[7] Center point coordinate actual value in the 1st axis of the plane of the 1st sphere Center point coordinate actual value in the 2nd axis of the plane of the 1st sphere Center point coordinate actual value in the 3rd axis of the plane of the 1st sphere _OVR[8] Sphere diameter difference of the 1st sphere mm mm mm mm mm mm mm Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 203

202 3.3 Measure workpiece (milling) Parameters Description Unit _OVR[9] _OVR[10] _OVR[11] Center point coordinate difference in the 1st axis of the plane of the 1st sphere Center point coordinate difference in the 2nd axis of the plane of the 1st sphere Center point coordinate difference in the 3rd axis of the plane of the 1st sphere _OVR[12] Sphere diameter actual value of 2nd sphere mm _OVR[13] _OVR[14] _OVR[15] Center point coordinate actual value in the 1st axis of the plane of the 2nd sphere Center point coordinate actual value in the 2nd axis of the plane of the 2nd sphere Center point coordinate actual value in the 3rd axis of the plane of the 2nd sphere _OVR[16] Sphere diameter difference of the 2nd sphere mm _OVR[17] _OVR[18] _OVR[19] Center point coordinate difference in the 1st axis of the plane of the 2nd sphere Center point coordinate difference in the 2nd axis of the plane of the 2nd sphere Center point coordinate difference in the 3rd axis of the plane of the 2nd sphere _OVR[20] Sphere diameter actual value of 3rd sphere mm _OVR[21] _OVR[22] _OVR[23] Center point coordinate actual value in the 1st axis of the plane of the 3rd sphere Center point coordinate actual value in the 2nd axis of the plane of the 3rd sphere Center point coordinate actual value in the 3rd axis of the plane of the 3rd sphere _OVR[24] Sphere diameter difference of the 3rd sphere mm _OVR[25] _OVR[26] _OVR[27] Center point coordinate difference in the 1st axis of the plane of the 3rd sphere Center point coordinate difference in the 2nd axis of the plane of the 3rd sphere Center point coordinate difference in the 3rd axis of the plane of the 3rd sphere _OVR[28] Safe area mm _OVI[0] WO number - _OVI[2] Measuring cycle number - _OVI[5] Probe number - _OVI[9] Alarm number - _OVI[11] Status offset request - _OVI[12] Supplementary error data for alarm, internal measurement evaluation - mm mm mm mm mm mm mm mm mm mm mm mm mm mm mm 204 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

203 3.3 Measure workpiece (milling) D - angular deviation spindle (CYCLE995) Function With this measuring method the angularity of a spindle to the machine tool is measured on a calibration ball. The measurement is carried out by combining the measuring methods "sphere" (CYCLE997) and "outer circle segment" (CYCLE979). Based on the measured values, the angular deviation of the spindle to the axis of the plane is calculated. With the measured angular deviations, the spindle can be mechanically aligned parallel to the tool axis or the corresponding tables for sag compensation can be updated. If there are rotary axes, the determined angular data can be used to align the rotary axis. To do this, the result parameter (_OVR) of CYCLE995 must be used. Measuring principle The 1st measurement of the calibration ball is performed with CYCLE997 and measurement is repeated. The starting angle can be freely selected. The incremental angle between the measuring points should be set to 90 degrees. From two measuring points along the circumference and one measuring point at the "north pole" of the sphere (highest point), the center point (position of the ball) is determined. In addition, the diameter of the calibration ball can be determined. The 2nd measurement is performed with CYCLE979 at the shaft of the probe at the distance of DZ. The starting angle and the incremental angle are taken from the 1st measurement. The measuring path and the safe area are also from the 1st measurement times a factor of 1.5. The center point of the probe shaft in the plane is determined. For both measurements, the switching direction of the probe is corrected for each individual measurement. The angular deviation in XY is calculated from the results of the two center points in XY and the distance between the two measurements in Z (for G17). The tolerance parameter of the angular values is optionally checked (dimensional tolerance "yes"). Note: The cycle CYCLE995 is based on the Renishaw AxiSet TM method based on the patent application, WO A1. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 205

204 3.3 Measure workpiece (milling) It is recommended to use the Renishaw probe with maximum accuracy for the application of the CYCLE995. Measure: Angular deviation, spindle (CY CLE995), 1st measurement Measure: Angular deviation, spindle (CY CLE995), 2nd measurement Requirements The precision of the calibration ball should be better than mm. An electronic program is loaded into the spindle with the longest possible stylus tip (>100 mm). The probe shaft should have a good surface quality (e.g. ground steel shaft). Starting position before the measurement Before the cycle is called, the probe must be positioned at the distance of the measuring path (DFA) above the mounted calibration ball (North Pole) so that this can be approached without any collisions at the circumference (equator). Position after the end of the measuring cycle The probe is located after the measuring cycle at the start position. In the probe direction (for G17 Z), the probe is at the distance of the measuring path (DFA) above the north pole. 206 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

205 3.3 Measure workpiece (milling) Procedure The part program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "3D" softkey. 3. Press the "Spindle angular displacement" softkey. The input window "Measure: Spindle angular deviation" opens. Parameter G code program Parameter Description Unit PL Measuring plane (G17 - G19) - Det. sphere diam. Calibration data set (1-12) - Determining the sphere diameter No Yes Sphere diameter mm α0 Contact angle Degrees DZ Depth infeed for 2nd measurement mm DFA Measurement path mm TSA Safe area for the measurement result mm Dimensional tolerance TUL Use dimensional tolerance Yes No Workpiece upper tolerance limit (incremental to the setpoint, only for dimensional tolerance "Yes") 1) Other parameters and correction targets can be set in the general SD 54760$SNS_MEA_FUNCTION_MASK_PIECE. - - mm Machine manufacturer Please observe the machine manufacturer s instructions. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 207

206 3.3 Measure workpiece (milling) List of the result parameters The measuring variant "machine geometry" provides the following result parameters: Table 3-29 Result parameter "Machine geometry" (CYCLE995) Parameters Description Unit _OVR [2] Actual angle between X and Z (X = 1st axis of the plane for G17, Z = 3rd axis of the plane for G17) Degrees _OVR [3] Actual angle between Y and Z (Y = 2nd axis of the plane for G17) Degrees _OVR [4] _OVR [5] _OVR [6] Distance in Z between the probe ball and measuring position at the probe shaft Exceeding the tolerance between X and Z (for dimensional tolerance "Yes") Exceeding the tolerance between Y and Z (for dimensional tolerance "Yes") _OVR [7] Spindle camber in XZ (XZ for G17) mm _OVR [8] Spindle camber in YZ (YZ for G17) mm _OVR [9] Upper tolerance limit of the measured angle values (_OVR[2], _OVR[3]) mm _OVI [2] Measuring cycle number - _OVI [3] Measuring version - _OVI [5] Number, probe calibration data field - _OVI [9] Alarm number - mm mm mm Table 3-30 Intermediate results 1st measurement (calibration ball) Parameters Description Unit _OVR [10] Setpoint calibration ball mm _OVR [11] Setpoint center point coordinate, 1st axis of the plane mm _OVR [12] Setpoint center point coordinate, 2nd axis of the plane mm _OVR [13] Setpoint center point coordinate, 3rd axis of the plane mm _OVR [14] Actual ball diameter mm _OVR [15] Actual value center point coordinate, 1st axis of the plane mm _OVR [16] Actual value center point coordinate, 2nd axis of the plane mm _OVR [17] Actual value center point coordinate, 3rd axis of the plane mm _OVR [18] Ball diameter difference mm _OVR [19] Difference center point coordinate, 1st axis of the plane mm _OVR [20] Difference center point coordinate, 2nd axis of the plane mm _OVR [21] Difference center point coordinate, 3rd axis of the plane mm 208 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

207 3.3 Measure workpiece (milling) Table 3-31 Intermediate results 2nd measurement (measuring probe shaft or 2nd probe ball at the shaft) Parameters Description Unit _OVR [22] Setpoint calibration ball diameter mm _OVR [23] Center point setpoint in the 1st axis of the plane mm _OVR [24] Center point setpoint in the 2nd axis of the plane mm _OVR [25] Center point actual value in the 1st axis of the plane degrees _OVR [26] Center point actual value in the 2nd axis of the plane degrees _OVR [27] Center point difference in the 1st axis of the plane Degrees _OVR [28] Center point difference in the 2nd axis of the plane degrees D - kinematics (CYCLE996) Function With the "Measure kinematics" measuring method (CYCLE996), it is possible to calculate the geometric vectors used to define the kinematic 5-axis transformation (TRAORI and TCARR) by measuring the ball position in space. The measurement is essentially carried out by means of workpiece probes which scan three positions of a measuring ball on each rotary axis. The ball positions can be defined in accordance with user specifications so that they correspond to the geometric ratios on the machine. The only way of setting the ball positions is to reposition the rotary axis that is to be measured in each case. Aside from the basic mechanics of the machine, no specific knowledge is required to use CYCLE996. No dimension drawings or machine location diagrams are necessary to carry out measuring. References: /PGZ/ Programming Manual SINUMERIK 840D sl/840d/840di sl Cycles, CYCLE800. Possible fields of application The measuring method "Measure kinematics" can be used to determine transformationrelevant data for kinematic transformations that contain rotary axes (TRAORI, TCARR). Redetermination of swivel data records Machine start-up Use of swivel-mounted workholders as TCARR Check of swivel data records Service following collisions Checking the kinematics during machining Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 209

208 3.3 Measure workpiece (milling) Kinematics with manual axes (manually adjustable rotary tables, swivel-mounted workholders) can be measured in the same way as kinematics with NC-controlled rotary axes. When starting CYCLE996 a swivel data record must be parameterized with the basic data (kinematic type, see the Programming Manual SINUMERIK 840D sl/840d/840di sl Cycles, CYCLE800). The measurement itself must be carried out without an active kinematic transformation. Requirements The following requirements must be met in order to use CYCLE996 (Measure kinematics): Calibrated 3D probe (probe type 710). Mounted calibration ball. Oriented tool carrier has been set-up (general MD 18088: $MN_MM_NUM_TOOL_CARRIER > 0) The basic geometry of the machine (X, Y, Z) is rectangular and referenced. The right angle refers to the workpiece spindle and should be preferably checked using a test mandrel or with the CYCLE995 measuring cycle. Defined position of the rotary axes involved in the transformation. Defined traverse directions in compliance with the standard of all axes involved in the transformation according to ISO and/or DIN (right-hand rule). Linear and rotary axes must have their optimum dynamic settings. This applies especially, when the machine is to perform tool orientations during machining with active TRAORI. The probe must be calibrated precisely. The calibrated tool length of the probe is included directly in the calculated vectors of the kinematics. When measuring, the measuring method "Circling around the calibration ball with tracking of the switching direction" should be used. Measuring principle The "Measure kinematics" measuring method always requires the following procedure: 1. Measure a rotary axis (Page 0 ) 2. Measure a second rotary axis (if this exists) 3. Calculate the swivel data records (calculate kinematics) (Page 0 ) 4. Automatic or user-supported activation of the calculated data The user (preferably the machine manufacturer) should ensure compliance with the specified sequence. If the position of the calibration ball within the machine can be specified as an inherent part of the design, then it will be possible to store the entire kinematic measurement process (carried out using CYCLE996) as a part program, which is extremely advantageous. As a result, the user can carry out measurement of the kinematics under a set of predefined conditions at any given point in time. 210 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

209 3.3 Measure workpiece (milling) The measurement of the rotary axis must be performed in the basic system of the machine. Metric machine with G710 and positions in mm. "INCH" machine with G700 and positions in INCHES. Measure: Kinematic (CYCLE996), 1st measurement, swivel table Measure: Kinematic (CYCLE996), 3rd measurement, swivel head Measuring kinematics Starting from the kinematics initial state, the relevant rotary axes are measured individually. Rotary axes 1 or 2 can be measured in any order. If the machine kinematics only have one rotary axis, this is measured as rotary axis 1. The basic data for the kinematics is always the data of the tool carrier with orientation capability. If a dynamic 5-axis transformation is to be supported, it is preferable to use transformation type 72 (vectors from TCARR data). The linear and rotary axes must be prepositioned at starting positions P1 to P3 before measuring cycle CYCLE996 is called in the NC program. The starting position is automatically accepted in CYCLE996 as the position setpoint for the "Measure ball" function. In each of the ball (rotary axis) positions selected, measuring is performed in accordance with the parameters and by calling CYCLE996. The kinematics are calculated using a separate, parameterized call of CYCLE996. When the 3rd measurement has been completed, the results of the measurement and the CYCLE996 setting "Calculate kinematics" are written to the _OVR[ ] result parameter. When the "Enter vectors" function is selected (refer to S_MVAR, S_TC), then data is output to the swivel data record that has been set-up (TCARR, TRAORI(1)). A protocol file with the measurement results in an appropriate data format (machine data or TCARR data) can be optionally output. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 211

210 3.3 Measure workpiece (milling) Note Requirements for measuring the kinematics with active TRAORI or active TCARR SD 55740: Set $SCS:MEA_FUNCTION_MASK, bit 8 = 1 Data record (swivel data or machine data) of the kinematics must be set up roughly (±1 mm). The probe must be positioned perpendicular on the measuring plane at the individual measuring points of the rotary axes. This can be performed with the swivel function (CYCLE800) or by positioning the rotary axes with TRAORI and then TOROT (for G17). Input screen forms "kinematics" CYCLE996 has to be called three times in order to complete the entire measuring and vector calculation process for one rotary axis. Between cycle calls, the user must reposition the rotary axis to be measured. Any rotary axis that is not being measured must not be repositioned during the measurement procedure. The linear axes are positioned at the starting positions P1, P2, P3. Using the respective softkeys, the 1st up to the 3rd measurement are called. At the end of the 3rd measurement, a call calculates the vectors of the measured rotary axis. The requirement for this is that the 1st to 3rd measurements have been carried out for the respective rotary axis, and that the corresponding measurement results (center points of the calibration ball) have been saved. The vectors of the machine kinematics are then calculated in full when both rotary axes have been measured. The measurement counter, parameter _OVR[40], is displayed in the result bit or in the protocol. Measurement for kinematics with swivel head: 1st measurement P1 (initial state) 2nd measurement P2 3rd measurement P3 With the 2nd and 3rd measurements, the rotary axis to be measured is rotated around the largest possible angle. The calibration ball position must be stationary during the measurements. Starting position before the measurement A rotary axis is measured by calling CYCLE996 three times (measurements 1 to 3). The probe ball must be able to reach the equator of the calibration ball. The 1st measurement must take place in the kinematics normal position. If a rotary axis rotates parallel to the spindle 212 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

211 3.3 Measure workpiece (milling) without offset in a head kinematics (fork head), the 1st measurement can be made with applied probe. The rotary axis that is not to be measured is not in the initial position of the kinematics. The starting position of the probe must be approached by the user or from the user program (see example program). The probe must be prepositioned in the direction of the tool orientation (ORI) above the highest point of the calibration ball (probe aligned with ball center point). After approaching the starting position, the distance (D) from the calibration ball should be as short as possible. Position after the end of the measuring cycle After each measurement (1 to 3) of a rotary axis, the probe is located above the calibration ball at a maximum distance of the measurement path DFA. Measuring an individual rotary axis The following steps must be carried out in order to measure a rotary axis: Mount the calibration ball on the machine table (user) Define and approach the three ball positions with the rotary axis that is to be measured (user) Specify and approach the three ball positions with the probe in a linear movement/in linear movements (user) Using CYCLE996, scan all three ball positions of the calibration ball with the probe. Mounting the calibration ball In the case of machinery, the calibration ball is to be installed on the machine table. In order to measure kinematics for swivel-mounted workholders, the ball must be incorporated into the appropriate workholder. In all cases it must be ensured that the probe can approach and bypass the mounted calibration ball without collision in all the selected rotary axis positions. Considering the need to avoid collisions, the calibration ball should be mounted as far as possible from the center of rotation of the rotary axis that is to be measured. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 213

212 3.3 Measure workpiece (milling) If the three ball positions result in too small a triangle, this will negatively affect the accuracy of the procedure: Calibration ball mounted sufficiently far from the center of rotation; large triangle can be clamped Calibration ball mounted too near the center of rotation; clamped triangle is too small Note While measuring a rotary axis, the mechanical hold-down of the calibration ball must not be altered. It is only with table and mixed kinematics that different calibration ball mounting positions are permissible for the purpose of measuring the first and subsequent rotary axes. Defining the rotary axis positions Three measuring points (ball position) must be defined for each rotary axis. Please note that the positions of the ball in space (resulting from the three defined rotary axis positions) should lead to as large a triangle as possible being clamped. Rotary axis positions sufficiently far away from one another; large triangle clamped Rotary axis positions poorly selected; clamped triangle is too small 214 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

213 3.3 Measure workpiece (milling) The calculated inside angle of the rotary axis angle segment is monitored in the TVL parameter. Angle values of < 20 degrees can cause inaccuracies when calculating the kinematics. Approaching the ball position First of all, the probe must be positioned above the calibration ball at each of the three rotary axis positions defined by the user. The position must only be approached by traversing the linear axes (X, Y, Z). The positions themselves must be entered (set up) by the user. They should be determined manually using an active probe. When selecting approach positions, please bear in mind that, within the context of automatic calibration ball scanning, the probe always moves in its preferred direction. Particularly where head and mixed kinematics are concerned, the starting position should be selected in a way that ensures alignment of the probe with the center point of the calibration ball in the approach position. Starting position selected directly above the calibration ball Starting position selected laterally above the calibration ball Note If the machine does not proceed as expected when the calibration ball is being scanned, the basic orientation and travel direction of the rotary axes should be checked. (Has DIN conformity been maintained when defining the axes?) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 215

214 3.3 Measure workpiece (milling) Starting position The probe must be prepositioned in the direction of the tool orientation (ORI) above the highest point of the calibration ball (probe aligned with ball center point). The distance (A) to the calibration ball after approaching the starting position should correspond to the measuring path parameter (DFA). Image 3-18 Starting position for the tool length in relation to the probe ball circumference Note Measuring the kinematics is also possible with active 5-axis transformation (TRAORI). As a requirement for measuring the kinematics with active TRAORI, the vectors of the 5-axis transformation must be roughly set. The positions for measuring the kinematics are approached in the user program with active transformation. The transformation can be switched on or off during the actual measuring. SD55740 $SCS_MEA_FUNCTION_MASK Bit 8 = 0 Measure kinematics without active TRAORI or TCARR Bit 8 = 1 Measure kinematics with active TRAORI or TCARR Measuring an individual ball position Once the probe has been positioned in accordance with user specifications above the ball, either manually or by the part program (starting point of CYCLE996), the calibration ball is scanned by calling CYCLE996 and the current ball position is measured. To this end, the user should parameterize and call CYCLE996 separately for each ball position. Calculating and activating the swivel data sets After measuring the three ball positions that are required in each case for all the relevant rotary axes, the entire set of swivel data sets can be calculated by means of CYCLE996. CYCLE996 should be parameterized and called for this purpose. 216 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

215 3.3 Measure workpiece (milling) Correction target In the "Calculate kinematics" screen form, in the "offset target" field, for the vectors it can be set as to whether "only" a calculation should be made (only measuring) or whether the calculated vectors should be saved in the swivel data set. Before saving, the user can decide whether the calculated swivel data set should be displayed and changed. If the calculated swivel data set should not be displayed, the user can decide whether the swivel data set should be immediately overwritten. In all other cases, before saving the swivel data set, the operator is prompted to make a selection. Table 3-32 Display options in the "Calculate kinematics" screen form Parameter Measuring only Swivel data set Display data set Yes No No Yes Data set can be edited Yes/no Confirm the change - - Yes/no - - entry field is not displayed In addition, the swivel data set can be saved as data file ("save data set"). The data file is saved in the actual NC data path (or workpiece) in which the measurement program is running. The file name corresponds to the name of the swivel data set, and is generated with a count index "_M1" to "_M99". The data file contains the syntax of the parameters of the swivel data set of the NC function TCARR, e.g. : $TC_CARR1[1]= $TC_CARR2[1]= ;I1xyz. If a transformation type <> 72 is set in the machine data for the dynamic transformation (TRAORI), the calculated vectors are saved in the protocol file also as machine data. Saving the log file When calculating the kinematics, before calling CYCLE996, the log cycle (CYCLE150) can be called. A log file is created with the measured and calculated vectors of the kinematics. Tolerance limits Activating tolerance limits when parameterizing CYCLE996 (compare Starting values calculated values), allows conclusions to be drawn regarding unusual changes in the mechanical kinematic chain. The unintentional automatic overwriting of starting values can be avoided by adjusting the tolerance limits. Note The rotary axis vectors V1/V2 (orientation of the rotary axes) are never automatically overwritten. Primarily, the calculated rotary axis vectors enable an assessment to be made regarding the mechanical desired/actual state of the kinematics. Depending on the kinematics configuration, Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 217

216 3.3 Measure workpiece (milling) even the smallest and corrected deviations in the position of the rotary axis vectors can result in large compensating movements. Normalizing = setting a fixed value Through normalizing, a new fixed value can be calculated in an axis direction (XYZ) for each rotary axis. This is required particularly for table kinematics because the result of the kinematics calculation refers to the height of the calibration ball. For example, with the normalizing, the Z component can be calculated to the reference point of the workpiece table. In head kinematics, the initial state of the 1st measurement of rotary axis 2 (if available, otherwise rotary axis 1) is calculated during the calculation of the kinematics. Normalizing is therefore usually not required for head kinematics. With orthogonal machine kinematics, the normalizing of a rotary axis only makes sense for a specific axis direction. Example: Table kinematics Rotary axis 2(C) rotates around Z -> normalizing of rotary axis 2(C) in axis direction Z makes sense. With normalizing "Yes", the value of the normalizing (fixed value) is written to the following linear vectors: Rotary axis 1 Rotary axis 2 Head kinematics I1 I3 Table kinematics I2 I4 Mixed kinematics I2 I4 Example: Table kinematics, rotary axis 1(A) rotates around X, rotary axis 2(C) rotates around Z. Normalizing of rotary axis 1(A) X=100 -> I2x=100 Normalizing of rotary axis 2(Z) Z=0 -> I4z=0 Note Normalizing (setting a fixed value) the vectors when measuring the kinematics SD55740: $SCS_MEA_FUNCTION_MASK/ Bit 7 (corresponded to _CHBIT[29] activated) Bit 7 = 0: Normalizing on the basis of the calculated orientation vectors (V1xyz, V2xyz) Bit 7 = 1: Normalizing on the basis of the orientation vectors entered in the swivel data set (TCARR) or with TRAORI, in the machine data. It is recommended that SD55740 bit 7 = 1 be set, as a machine test has proved that this further improves the accuracy of the calculated offset vectors. 218 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

217 3.3 Measure workpiece (milling) Procedure The part program to be processed has been created and you are in the editor. 1. Press the "Meas. workpiece" softkey. 2. Press the "3D" softkey. 3. Press the "Kinematics" softkey. The "Measure: Kinematic" input window opens. You can then open the following input windows via the following softkeys: 1. Measurement 2. Measurement 3. Measurement (see Parameters of 1st to 3rd measurement (Page 0 )) Calculate (see Calculate parameters (Page 0 )) Parameters of 1st to 3rd measurement G code program Parameter Description Unit PL Measuring plane (G17 - G19) - Positioning Align probe (only for positioning "On circular path") Calibration data set (1-12) - Traverse around sphere: Parallel to the axis On circular path Always align probe 2) in the same contact direction: Yes No 2) Rotary axis 1 Name of rotary axis 1 of the swivel data set - Rotary axis angle 1 Rotary axis angle during the measurement 1) Degrees Rotary axis 2 Name of rotary axis 2 of the swivel data set - Rotary axis angle 2 Rotary axis angle during the measurement 1) Degrees Ball diameter mm α0 Starting angle (only for "positioning on circular path") Degrees DFA Measurement path mm TSA Safe area for the measurement result mm 1) Only for manual or semi-automatic rotary axis of the swivel data set 2) Note: Preferably the measuring method "Positioning on circular path" and "Align probe in contact direction" should be used for the best measurement results. - - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 219

218 3.3 Measure workpiece (milling) Calculate parameters G code program Parameter Description Unit PL Measuring plane (G17 - G19) - Correction target Only measuring (only calculate vectors) Swivel data set (calculate vectors and save to swivel data set) Display data set Yes/No No Yes - Data set can be changed - - Yes/No - - Confirm the change - Yes/No - - Save data set Data set is saved in a protocol file Rotary axis 1 Name of rotary axis 1 of the swivel data set - Normalizing No (without normalizing) X (normalizing in direction X) Y (normalizing in direction Y) Z (normalizing in direction Z) Value input Position value for normalizing mm Rotary axis 2 Name of rotary axis 2 of the swivel data set - Normalizing No (without normalizing) X (normalizing in direction X) Y (normalizing in direction Y) Z (normalizing in direction Z) Value input Position value for normalizing mm Tolerance Use dimensional tolerance Yes No TLIN Max. tolerance of the offset vectors (only for tolerance "Yes") mm TROT Max. tolerance of the rotary axis vectors (only for tolerance "Yes") Degrees TVL Limit value of the minimum inside angle of the measured triangle of the three measurements of the rotary axis (see "Mounting the calibration" above). Close vector chain Yes for kinematics mounted permanently on the machine - entry field is not displayed No for changeable kinematics (e.g. interchangeable heads) Degrees - Note TVL With TVL values < 20 degrees, scattering of the measured values can result in inaccuracies in the calculation of the kinematics. 220 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

219 3.3 Measure workpiece (milling) List of the result parameters The measuring method "Calculate kinematics" provides the following result parameters: Table 3-33 "Calculate kinematics" result parameters Parameter Description Unit _OVR[1] Offset vector I1 $TC_CARR1[n] X component mm _OVR[2] Offset vector I1 $TC_CARR2[n] Y component mm _OVR[3] Offset vector I1 $TC_CARR3[n] Z component mm _OVR[4] Offset vector I2 $TC_CARR4[n] X component mm _OVR[5] Offset vector I2 $TC_CARR5[n] Y component mm _OVR[6] Offset vector I2 $TC_CARR6[n] Z component mm _OVR[7] Rotary axis vector V1 $TC_CARR7[n] X component _OVR[8] Rotary axis vector V1 $TC_CARR8[n] Y component _OVR[9] Rotary axis vector V1 $TC_CARR9[n] Z component _OVR[10] Rotary axis vector V2 $TC_CARR10[n] X component _OVR[11] Rotary axis vector V2 $TC_CARR11[n] Y component _OVR[12] Rotary axis vector V2 $TC_CARR12[n] Z component _OVR[15] Offset vector I3 $TC_CARR15[n] X component mm _OVR[16] Offset vector I3 $TC_CARR16[n]Y component mm _OVR[17] Offset vector I3 $TC_CARR17[n] Z component mm _OVR[18] Offset vector I4 $TC_CARR18[n] X component mm _OVR[19] Offset vector I4 $TC_CARR19[n] Y component mm _OVR[20] Offset vector I4 $TC_CARR20[n] Z component mm _OVI[2] Measuring cycle number - _OVI[3] Measuring method (S_MVAR) - _OVI[8] Number of swivel data set (S_TC) - _OVI[9] Alarm number - The measurement results (calculated vectors) depend on the type of kinematics Kinematics type Head kinematics 1) I1 $TC_CARR1...3[n] I2 $TC_CARR4...6[n] I3 $TC_CARR [n] Table kinematics 2) I2 $TC_CARR4...6[n] I3 $TC_CARR [n] I4 $TC_CARR [n] Mixed kinematics 3) Corresponds to Corresponds to Measuring result _OVR[1]..._OVR[3] _OVR[4]..._OVR[6] _OVR[15]..._OVR[17] _OVR[18]..._OVR[20] = 0 _OVR[4]..._OVR[6] _OVR[15]..._OVR[17] _OVR[18]..._OVR[20] _OVR[1]..._OVR[3] = 0 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 221

220 3.3 Measure workpiece (milling) Kinematics type I1 $TC_CARR1...3[n] I2 $TC_CARR4...6[n] I3 $TC_CARR [n] I4 $TC_CARR [n] Corresponds to Measuring result _OVR[1]..._OVR[3] _OVR[4]..._OVR[6] _OVR[15]..._OVR[17] _OVR[18]..._OVR[20] The result parameters that are not calculated = 0 1) Close vector chain I1=-(I3+I2); for fixed-mounted machine kinematics 2) Close vector chain I4=-(I3+I2); for fixed-mounted machine kinematics 3) Close vector chain I1=-I2 I4=-I3; for fixed-mounted machine kinematics Table 3-34 Intermediate results _OVR[32] to _OVR[71] Parameter Description Unit _OVR[32,33,34] 1) Linear vector of 1st rotary axis is not normalized mm _OVR[35,36,37] 1) Linear vector of 2nd rotary axis is not normalized mm _OVR[40] 2) Measurement counter x0 = 1st measurement of 1st rotary axis started x1 = 1st measurement of 1st rotary axis is OK x2 = 2nd measurement of 1st rotary axis is OK x3 = 3rd measurement of 1st rotary axis is OK 0x = 1st measurement of 2nd rotary axis started 1x = 1st measurement of 2nd rotary axis is OK 2x = 2nd measurement of 2nd rotary axis is OK 3x = 3rd measurement of 2nd rotary axis is OK 33 = Both rotary axes measured _OVR[41,42,43] 2) 1. measurement of 1st rotary axis mm _OVR[44,45,46] 2) 2. measurement of 1st rotary axis mm _OVR[47,48,49] 2) 3. measurement of 1st rotary axis mm _OVR[50] Tool length of the probe mm _OVR[51,52,53] 2) 1. measurement of 2nd rotary axis mm _OVR[54,55,56] 2) 2. measurement of 2nd rotary axis mm _OVR[57,58,59] 2) 3. measurement of 2nd rotary axis mm _OVR[60,61,62] Measuring positions, rotary axis 1 for 1st, 2nd, 3rd measurement Degrees _OVR[63,64,65] Measuring positions, rotary axis 2 for 1st, 2nd, 3rd measurement Degrees _OVR[66,67,68] Active rotation of the WO for 1st measurement of rotary axis 1 in XYZ _OVR[69,70] Reserved - _OVR[71] _OVR[72,73,74] _OVR[75,76,77] _OVR[98] Actual calibration ball diameter from the 1st measurement of rotary axis 1 Actual calibration ball diameter of the 1st, 2nd, 3rd measurement rotary axes 1 Actual calibration ball diameter of the 1st, 2nd, 3rd measurement rotary axes (if there is a rotary axis) (see note regarding SD55644 $SCS_MEA_KIN_DM_TOL) Vector V1x after calculating as unit vector (without user-specific normalization) - Degrees mm mm mm 222 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

221 3.3 Measure workpiece (milling) Parameter Description Unit _OVR[99] Vector V1y after calculating as unit vector _OVR[100] Vector V1z after calculating as unit vector _OVR[101] Vector V2x after calculating as unit vector (without user-specific normalization) _OVR[102] Vector V2y after calculating as unit vector _OVR[103] Vector V2z after calculating as unit vector 1) The linear vectors are assigned to the specific vectors of the kinematics (I1, I2, etc.) in accordance with the normalizing process. 2) Result parameters _OVR[41] up to _OVR[59] are saved in groups of 3. The values include the measured actual values of the 3 linear axes (XYZ) in the machine coordinate system MCS. At the start of the 1st measurement, the intermediate results (sphere center points) of the rotary axis are deleted. At 1st measurement of 1st rotary axis deletion of _OVR[41]... _OVR[49] At 1st measurement of 2nd rotary axis deletion of _OVR[51]... _OVR[59] Programming example ;Measure kinematics ;Mixed kinematics with a B axis around Y and C axis around Z (MIXED_BC). ;Calibration ball at 2*45 degrees, directly mounted on a table. ;WO in G56. Only the position of the calibration ball ;has to be specified in the initial state of the kinematics (B=0 C=0). ;Determine G56 with measuring spigot in the JOG mode and approach in XY, ;then set ball north pole Z=0. ;Swivel data must be entered according to the machine drawing dimensions -> _SDA _SDE. ;Intermediate positions are approached with active TRAORI. ;To do this, using the online tool offset TOFFL, the TCP ;is shifted to the center of the measuring ball. ;Measuring positions for MIXED_BC ;P1.. P3 rotary axis 1 ;P4.. P6 rotary axis 2 DEF REAL _P1[2]=SET(0,0) ;Measuring point P1 rotary axis 1(B), rotary axis 2(C) DEF REAL _P2[2]=SET(45,0) DEF REAL _P3[2]=SET(-45,0) DEF REAL _P4[2]=SET(0,0) DEF REAL _P5[2]=SET(0,90) DEF REAL _P6[2]=SET(0,180) DEF REAL _BALL=25 ;Calibration ball diameter DEF REAL _SAVB=1 ;Safety clearance above the calibration ball ;Globally pre-assign measuring parameters _FA=_SAVB*3 _TSA=_SAVB*4 REPEAT _SDA _SDE ;Read-in swivel data set Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 223

222 3.3 Measure workpiece (milling) MSG(" load transformation data. OK?? ") M0 STOPRE MSG() ;GOTOF _MCA ;Only calculate kinematics _OVR[40] to _OVR[71] OK G17 CYCLE800() ORIAXES ORIMKS TRAORI G56 T="3D-TASTER" D1 M6 IF (NOT $P_SEARCH) AND (NOT $P_ISTEST) AND (NOT $P_SIM) _OVR[40]=0 ;Zero the measuring counter ENDIF ; Measurement, rotary axis 1 N99 G1 G710 G90 Z30 FFWON F2000 TOFFL=_BALL/2+_SAVB D1 B=_P1[0] C=_P1[1] ;Kinematics initial state Z = _SAVB TOFFL=0 X0 Y0 ;Circle around the ball CYCLE996(10101,1,1,_BALL,0,0,0,0,0,0,0,0,_FA,_TSA,1,,1,) M1 STOPRE TOROT M1 Z=IC(-_FA+_SAVB) TOROTOF M1 ; Measurement, rotary axis 1 G1 F2000 TOFFL=_BALL/2+_SAVB ;When repositioning, correct the tool online B=_P2[0] C=_P2[1] TOFFL=0 ;Disable online correction again ;Circle around the ball, starting angle 45 degrees CYCLE996(10102,1,1,_BALL,45,0,0,0,0,0,0,0,_FA,_TSA,1,,1,) 224 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

223 3.3 Measure workpiece (milling) TOROT Z=IC(-_FA+_SAVB) ;Approach starting position TOROTOF ; measurement, rotary axis 1 G1 F2000 TOFFL=_BALL/2+_SAVB D1 B=_P3[0] C=_P3[1] TOFFL=0 CYCLE996(10103,1,1,_BALL,210,0,0,0,0,0,0,0,_FA,_TSA,1,,1,) TOROT Z=IC(-_FA+_SAVB) TOROTOF ; measurement, rotary axis 2 ;Initial state, 1st measurement, rotary axis 1 = 1st measurement, rotary axis 2 _OVR[51]=_OVR[41] _OVR[52]=_OVR[42] _OVR[53]=_OVR[43] _OVR[75] = _OVR[72] ;accept actual diameter IF (NOT $P_SEARCH) AND (NOT $P_ISTEST) AND (NOT $P_SIM) _OVR[40]=_OVR[40]+10 ENDIF ; Measurement, rotary axis 2 G1 F2000 TOFFL=_BALL/2+_SAVB D1 B=_P5[0] C=_P5[1] TOFFL=0 M1 CYCLE996(20102,1,1,_BALL,0,0,0,0,0,0,0,0,_FA,_TSA,1,,1,) TOROT Z=IC(-_FA+_SAVB) TOROTOF ; rd measurement, rotary axis 2 TOFFL=_BALL/2+_SAVB G1 D1 C=_P6[1] F2000 TOFFL=0 CYCLE996(20103,1,1,_BALL,_STA1,0,0,0,0,0,0,0,_FA,_TSA,1,,1,) TOROT Z=IC(-_FA+_SAVB) TOROTOF ENDIF G0 Z30 B0 C0 ; Calculate kinematics Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 225

224 3.3 Measure workpiece (milling) _MCA: ;Display data set. Save data set as protocol file ;Normalizing rotary axis 2(C) on Z=0 -> table upper edge CYCLE996( ,1,1,_BALL,_STA1,0,0,0,0,0.02,0.001,22,_FA,_TSA,1,,1,101) MSG("Kinematics measurement OK") M1 M30 ;end of program ; _SDA: ;Swivel data set according to machine drawing TCARR=0 TRAFOOF TCARR=0 $TC_CARR1[1]=-25 $TC_CARR2[1]=0 $TC_CARR3[1]=-121 ;I1xyz $TC_CARR4[1]=25 $TC_CARR5[1]=0 $TC_CARR6[1]=121 ;I2xyz $TC_CARR7[1]=0 $TC_CARR8[1]=1 $TC_CARR9[1]=0 ;V1 axis B around Y $TC_CARR10[1]=0 $TC_CARR11[1]=0 $TC_CARR12[1]=-1 ;V2 axis C around Z $TC_CARR13[1]=0 $TC_CARR14[1]=0 $TC_CARR15[1]=0 $TC_CARR16[1]=0 $TC_CARR17[1]=0 ;I3xyz $TC_CARR18[1]=0 $TC_CARR19[1]=0 $TC_CARR20[1]=0 ;I4xyz $TC_CARR23[1]="M" $TC_CARR24[1]=0 $TC_CARR26[1]=0 $TC_CARR28[1]=0 $TC_CARR25[1]=0 $TC_CARR27[1]=0 $TC_CARR29[1]=0 $TC_CARR30[1]=-92 $TC_CARR31[1]=0 $TC_CARR32[1]=92 $TC_CARR33[1]=360 STOPRE NEWCONF _SDE: 226 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

225 3.3 Measure workpiece (milling) Expanded functionality CYCLE Checking the sphere diameter When measuring the calibration sphere ( measurement) the measured diameter (actual diameter) of the calibration sphere is saved to the following result parameters: _OVR[72] to _OVR[74] _OVR[75] to _OVR[77] Actual calibration sphere diameter measurement rotary axis 1 Actual calibration sphere diameter measurement rotary axis 2 (if a rotary axis exists) When setting data $SCS_MEA_KIN_DM_TOL > 0, after the 1st measurement and when calculating the kinematics, the measured calibration sphere diameter is checked. If the deviation is greater than in setting data $SCS_MEA_KIN_DM_TOL, fault or is output rotary axis 1: Tolerance, diameter calibration sphere between measurement %4 exceeded rotary axis 2: Tolerance, diameter calibration sphere between measurement %4 exceeded Scaling of rotary axis vectors V1 and V2 When calculating the kinematics, the vectors can be calculated as unit vector or as a userspecific vector. For user-specific rotary axis vectors, a vector component is always 1 or -1. The two remaining vector components are appropriately converted using a factor. The function is activated using setting data $SCS_MEA_FUNCTION_MASK, bit 9. Example: Swivel head with 45 degrees rotary axis 1. Vector V2xyz as unit vector calculating the kinematics (SD55740, bit 9=0): $TC_CARR10[1] = $TC_CARR11[1] = EX-06 $TC_CARR12[1] = Vector V2xyz user-specific after calculating the kinematics (SD55740, bit 9=1) $TC_CARR10[1] = $TC_CARR11[1] = EX-06 $TC_CARR12[1] = 1 If SD55740, bit 9=1 is set, for comparison purposes, vectors V1 and V2 are saved in the result parameters _OVR[98] up to _OVR[103] before calculating the user-specific scaling. Result parameters _OVR[98] to _OVR[103] are also written to the measuring data file. _OVR[98] _OVR[99] Vector V1x after calculating as unit vector (without user-specific normalization) Vector V1y after calculating as unit vector _OVR[100] Vector V1z after calculating as unit vector _OVR[101] Vector V2x after calculating as unit vector (without user-specific normalization) _OVR[102] Vector V2y after calculating as unit vector _OVR[103] Vector V2z after calculating as unit vector Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 227

226 3.3 Measure workpiece (milling) D measuring on machines with orientation transformation Function Measuring with active orientation transformation, i.e. with the swivel cycle CYCLE800 (orientable tool carrier TCARR), or with the kinematic 5-axis transformation (TRAORI) with the measuring cycles is possible. The probe must be positioned perpendicular to the machining plane or parallel to the tool axis before calling the measuring cycles. The Align plane (CYCLE998) and Measure kinematics (CYCLE996) functions are the exception. Here, the probe is always at an angle to the object to be measured. The workpiece measurement is generally based on the active workpiece coordinate system WCS. Checking the correct switching direction when measuring the workpiece If elements (hole, edge, etc.) are measured in the swiveled, rotated WCS, the switching direction of the 3D workpiece probe must be checked as follows during the first commissioning of the machine in the JOG and AUTO modes: Bit1 = 1 must be set in SD $SCS_MEA_FUNCTION_MASK (coupling of the spindle with the coordinate rotation). The switching direction in X+ (for G17) in the initial state of the machine kinematics must be marked accordingly on the probe. Using the measuring of a hole with CYCLE977 in the swiveled plane as an example, the marked switching direction must be aligned towards X+ when starting and probing the 1st measuring point. With active orientation transformation (TCARR, CYCLE800, TRAORI), the spindle position changed by the tool orientation is calculated internally in the measuring cycles and the spindle corrected accordingly. The result of the calculation is saved in the GUD variable _MEA_CORR_ANGLE[1]. The correct spindle position during measuring must be checked on the workpiece for different orientations of the object to be measured. After a successful check, SD $SCS_MEA_FUNCTION_MASK, bit1 = 0 can be set. The measurement results must correspond to those of the measurements with coupling of the spindle. 228 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

227 3.3 Measure workpiece (milling) Note Additional adaptation of the correction angle An additional adaptation of the correction angle for the positioning of the spindle may be required for the selected machine kinematics or applications. With the CUST_MEACYC.SPF manufacturer cycle, you can write the correction angles _MEA_CORR_ANGLE[0] and _MEA_CORR_ANGLE[1]. These angles affect the spindle position / probe orientation when measuring or the internal conversion of the trigger values if the spindle is not to be aligned in the switching direction (SD bit1 = 0, SPOS = 0 during measuring) Measuring the workpiece on a machine with combined technologies Measuring a workpiece on a milling/turning machine General This chapter refers to measuring a tool on milling/turning machines. Turning is set up as the 1st technology and milling as the 2nd technology. Preconditions: 1. Milling: MD52200 $MCS_TECHNOLOGY = 2 2. Turning: MD52201 $MCS_TECHNOLOGY_EXTENSION = 1 Further, the following setting data must be set: SD $SC_TOOL_LENGTH_TYPE = 3 SD $SC_TOOL_LENGTH_CONST = 17 SD $SC_TOOL_LENGTH_CONST_T = 19 Measuring workpieces using turning technology on a milling machine is realized using milling technology. For example, if the outer diameter of a contour is to be measured, then this can be realized using CYCLE977 "Measure spigot" at the G17 plane. If the measured values are to be corrected in a turning tool, then the programmer must specify the tool lengths L3x or L1z to be corrected, and possibly the sign of the correction. The selection of the correction depends on the turning tool orientation (align turning tool function beta and gamma) for turning. Please take into account SD55760 $SNS_MEA_FUNCTION_MASK_PIECE bit12 and bit13. It only makes sense to correct the measured values of the turned tool in a work offset for the Z axis. The machine manufacturer makes the correct setting of the turning center in XY when commissioning the machine. Note the machine manufacturer s instructions If the tool probe is to be reorientated for making the measurement, then this is realized using the swivel plane function (CYCLE800). Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 229

228 3.3 Measure workpiece (milling) Additional settings/notes relating to milling/turning technology should be taken from IM9 Chapter "Turning on milling machines". Function Using measuring cycles, the probe can be calibrated on milling/turning machines and milling, drilling and turning tools can be measured. A probe is calibrated using the CYCLE976 cycle Cycle CYCLE971 is used to measure milling and drilling tools Cycle CYCLE982 is used to measure turning tools The descriptions for the appropriate cycles in this manual should be used to parameterize the individual measuring versions Measuring a workpiece on a turning/milling machine The following section refers to the workpiece measuring on turning/milling machines. Whereby turning is set up as the 1st technology and milling as the 2nd technology. - Turning measurement (measure diameter, outside, inside, etc.) If measuring is to be performed in different tool orientations (B axis for turning technology), the probe can be prepositioned with the "Tool alignment" function (CYCLE800). - Milling measurement (measure hole, set edge, align edge, etc.) If measuring is to be performed in different tool orientations, the probe can be prepositioned with the "Swivel plane" function (CYCLE800). Value specifications of the transverse axis (X) of the measuring cycles under milling are performed in the radius (DIAMOF). The measuring cycles under milling also work internally with radius programming in relation to a transverse axis. With hole and spigot measurement (CYCLE977, CYCLE979), the object to be measured is specified in the diameter. The workpiece probe cannot be calibrated under the active G18 machining plane (turning) for turning/milling machines for geometric reasons. The workpiece measurements should be performed in G18 during turning. The probe is therefore calibrated under G17 or G19 and the trigger values allocated internally accordingly Allocating the trigger values Function As of SW 4.5 SP2, the following application is enabled with the "Calibrating and measuring in different machining planes" function: Calibrating (with CYCLE976) in the G17 or G19 working plane Workpiece measuring in G18 as for turning (with CYCLE974, CYCLE994) 230 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

229 3.3 Measure workpiece (milling) Requirement 1st turning technology: MD 52200$MCS_TECHNOLOGY = 1 2nd milling technology: MD 52201$MCS_TECHNOLOGY_EXTENSION = 2 Active tool is a 3D multi probe, type Uniformity when using a 3D probe of type 710 Function In accordance with the "Calibrating and measuring in different machining planes" function on a turning/milling machine, the 3D probe type (710) can be used for all workpiece measuring variants (turning and milling) on the basis of a calibration data set. Requirement Setting data SD $SC_TOOL_LENGTH_CONST = 18 (or -18) Setting data SD $SC_TOOL_LENGTH_TYPE = 2 Active tool is a 3D multi probe, type 710 Note If the above requirements are not satisfied for measuring under turning, alarm "Check tool type of the workpiece probe" is output. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 231

230 3.4 Measure tool (turning) 3.4 Measure tool (turning) General information The measuring cycles below are intended for use on turning machines. Note Spindle Spindle commands in the measuring cycles always refer to the active master spindle of the control. When using the measuring cycles at machines with several spindles, then the spindle involved must be defined as master spindle before the cycle call. References: /PG/ Programming Manual SINUMERIK 840D sl / 828D Fundamentals Plane definition The measuring cycles work internally with the 1st and 2nd axes of the actual plane G17 to G19. The default setting for lathes is G18. Note The measuring cycle for tool measurement, turning (CYCLE982) does not position in the 3rd axis (Y for G18). The user must position in the 3rd axis. 232 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

231 3.4 Measure tool (turning) Machine/workpiece-related measuring/calibrating Machine-related measuring/calibrating: Measuring is performed in the basic coordinate system (machine coordinate system with kinematics transformation disabled). The switching positions of the tool probe refer to the machine zero. Data from the following general setting data are used (PLUS and MINUS define the traversing direction of the tool): 1 SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX1 2 SD $SNS_MEA_TP_TRIG_PLUS_DIR_AX1 3 SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX2 4 SD $SNS_MEA_TP_TRIG_PLUS_DIR_AX Image 3-19 Tool probe, machine-related (G18) Workpiece-related measuring/calibrating: The switching positions of the tool probe refer to the workpiece zero. Data from the following general setting data are used (PLUS and MINUS define the traversing direction of the tool): 1 SD $SNS_MEA_TPW_TRIG_MINUS_DIR_AX1 2 SD $SNS_MEA_TPW_TRIG_PLUS_DIR_AX1 3 SD $SNS_MEA_TPW_TRIG_MINUS_DIR_AX2 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 233

232 3.4 Measure tool (turning) 4 SD $SNS_MEA_TPW_TRIG_PLUS_DIR_AX Image 3-20 Tool probe, workpiece-related (G18) Note Workpiece-related or machine-related measurement requires an appropriately calibrated tool probe, see ChapterCalibrate probe (CYCLE982) (Page 234). Compensation strategy The tool measuring cycle is intended for various applications: First measurement of a tool (general setting data SD $SNS_MEA_FUNCTION_MASK_TOOL Bit9): The tool offset values in geometry and wear are replaced. The offset is applied in the geometry component of the particular length. The wear component is deleted. Post measurement of a tool (general setting data SD $SNS_MEA_FUNCTION_MASK_TOOL Bit9): The resulting difference is calculated into the wear component (length) of the tool. Empirical values may optionally be included. A mean value is not calculated. See also Changes from cycle version SW4.4 and higher (Page 325) Calibrate probe (CYCLE982) Function This measuring version can be used to calibrate a tool probe. Using the calibration tool, the actual distances between machine or workpiece zero and the probe trigger points are determined. 234 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

233 3.4 Measure tool (turning) Values are corrected without empirical and mean values. Note If a special calibration tool is not available, a turning tool can be used instead with cutting edge positions 1 to 4 for the calibration of two sides of the probe. Measuring principle Calibrating with tool type calibration tool (type 585) The calibration tool is shaped (angled) in such a way that the probe can be calibrated on all four sides with it. Calibrating with tool type calibration tool (type 725) or turning tool (type 5xy) When a turning tool or a calibration tool, type 725, is used, the probe can only be calibrated from 2 sides. Calibrating the tool probe with a calibration toolcalibrating a tool probe with a turning tool The cycle positions the calibration or turning tool to the probe. With a cycle call, the switching position in the specified measuring axis and measuring direction is calibrated. Preconditions Lengths 1 and 2 and the radius of the calibration or turning tool must be known exactly and stored in a tool offset data record. This tool offset must be active when the measuring cycle is called. For calibration, a reference turning tool, type 5xy, with precisely known geometry or a type 585 or type 725 calibration tool can be used (type 580 3D probe turning cannot be used) Calibration with a calibration or turning tool with cutting edge positions 1 to 4 is possible. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 235

234 3.4 Measure tool (turning) The lateral surfaces of the probe cube must be aligned parallel to the machine axes Z1, X1 (axes of the plane). The approximate positions of the switching surface of the probe regarding the machine or workpiece zero must be entered before calibration starts in the general setting data (see Commissioning Manual SINUMERIK Operate (IM9) / SINUMERIK 840D sl, Chapter "Tool measurement in turning"). These values are used for automatic approach to the probe with the calibration tool and their absolute value must not deviate from the actual value by more than the value in parameter TSA. The probe must be reached within the total path 2 DFA. Starting position before the measurement Calibrating the tool probe with a calibration toolcalibrating a tool probe with a turning tool Cutting edge positions 1 to 4 and suitable approach positions for both axes (machine-related) 1 trigger point of the 1st measuring axis in the negative direction (general SD 54625) 2 trigger point of the 1st measuring axis in the positive direction (general SD 54626) 3 trigger point of the 2nd measuring axis in the negative direction (general SD 54627) 4 trigger point of the 2nd measuring axis in the positive direction (general SD 54628) The cycle handles the approach to the probe. 236 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

235 3.4 Measure tool (turning) Position after the end of the measuring cycle The calibration or turning tool is located by the measurement path away from the measuring surface Trigger point of the 1st measuring axis in the positive direction (general SD 54626) 2 Trigger point of the 1st measuring axis in the negative direction (general SD 54625) Image 3-21 Position after the end of the measuring cycle, example, 1st axis of the plane (for G18: Z) Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. tool" softkey. 2. Press the "Calibrate probe" softkey. The input window "Calibrate: Probe" opens. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 237

236 3.4 Measure tool (turning) Parameters G code program ShopTurn program Parameters Description Unit Parameters Description Unit F Calibration data set (1-6) - T Name of the calibration tool - Calibration and measuring feedrate Distance/ min D Cutting edge number (1-9) - F β V Z X Y Calibration data set (1-6) - Calibration and measuring feedrate Tool alignment with swivel axis (0 degrees) (90 degrees) Value entry Tool orientation with a tool spindle Start point Z of the measurement Start point X of the measurement Start point Y of the measurement mm/min Degrees Degrees mm mm mm Parameters Description Unit Measuring axis Measuring axis (for measuring plane G18) - X Z DFA Measurement path mm TSA Safe area for the measurement result mm List of the result parameters The measuring variant "Calibrate probe" provides the following result parameters: Table 3-35 "Calibrate probe" result parameters Parameters Description Unit _OVR[8] Trigger point in minus direction, actual value of 1st axis of the plane mm _OVR[10] Trigger point in plus direction, actual value of 1st axis of the plane mm _OVR[12] Trigger point in minus direction, actual value of 2nd axis of the plane mm _OVR[14] Trigger point in plus direction, actual value of 2nd axis of the plane mm _OVR[9] Trigger point in minus direction, difference of 1st axis of the plane mm _OVR[11] Trigger point in plus direction, difference of 1st axis of the plane mm _OVR[13] Trigger point in minus direction, difference of 2nd axis of the plane mm 238 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

237 3.4 Measure tool (turning) Parameters Description Unit _OVR[15] Trigger point in plus direction, difference of 2nd axis of the plane mm _OVR[27] Zero offset area mm _OVR[28] Safe area mm _OVI[2] Measuring cycle number - _OVI[3] Measuring variant - _OVI[5] Probe number - _OVI[9] Alarm number Turning tool (CYCLE982) Function With this measuring version, the tool length (L1 and/or L2) of a turning tool with cutting edge positions 1 to 8 can be determined. The measuring version checks whether the difference to be corrected with respect to the old tool length lies within a defined tolerance range: Upper limits: Safe area TSA and dimensional difference control DIF Lower limit: Work offset range TZL If this range is not violated, the new tool length is accepted in the tool offset, otherwise an alarm is output. Violation of the lower limit is not corrected. Measuring principle For "complete" measuring, all lengths of a turning tool are measured: Turning tool with cutting edge positions 1 to 4: L1 and L2 Turning tool with cutting edge position 5 or 7: L2 Turning tool with cutting edge position 6 or 8: L1 If the turning tool has a cutting edge position 1 to 4, contact is made with the probe in both axes of the plane (for G18 Z and X), whereby the measurement starts with the 1st axis of the plane (for G18 Z). For cutting edge positions 5 to 8, a measurement is only performed in one axis: Cutting edge position 5 or 7: 1st measuring axis for G18 Z Cutting edge position 6 or 8: 2nd measuring axis for G18 X. When measuring "axis by axis", the length of the turning tool in the parameterized measuring axis is measured. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 239

238 3.4 Measure tool (turning) Image 3-22 Measure: Turning tool (CYCLE982), example: Complete measuring Preconditions The tool probe must be calibrated, see Calibrate probe (CYCLE982) (Page 234). The approximate tool dimensions must be entered in the tool offset data: Tool type 5xx Cutting edge position, cutting edge radius Lengths in X and Z The tool to be measured must be active with its tool offset values when the cycle is called. Starting position before the measurement Before the cycle is called, the tool must be moved to the tool tip starting position, as shown in the following diagram. Image 3-23 Cutting edge positions 1 to 4 and suitable starting positions for both axes The center of the tool probe and the approach distance are calculated automatically and the required traversing blocks generated. The center of the cutting edge radius is positioned at the center of the probe. 240 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

239 3.4 Measure tool (turning) Image 3-24 Measuring the length of a turning tool: Offset by the cutting edge radius, example SL=3 Position after the end of the measuring cycle For an "axis by axis" measurement, the tool tip is the measurement path distance away from the probed measuring surface of the probe. For a "complete" measurement, after the measurement, the tool is positioned at the starting point before the cycle was called. Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. tool" softkey. 2. Press the "Turning tool" softkey. The input window "Measure: Turning tool" opens. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 241

240 3.4 Measure tool (turning) Parameters G code program ShopTurn program Parameters Description Unit Parameters Description Unit PL Measuring plane (G17 - G19) - T Name of the tool to be measured Calibration data set (1-6) - D Cutting edge number (1-9) - β V Z X Y Calibration data set (1-6) - Tool alignment with swivel axis: (0 degrees) (90 degrees) Value entry Tool orientation with a tool spindle Start point Z of the measurement Start point X of the measurement Start point Y of the measurement - Degrees Degrees mm mm mm Parameters Description Unit Measure Measure tool lengths (for measuring plane G18) - Complete (measure length Z and length X Only measure tool length Z Only measure tool length X DFA Measurement path mm TSA Safe area for the measurement result mm TZL Tolerance range for work offset mm TDIF Tolerance range for dimensional difference monitoring mm List of the result parameters The measuring variant "Turning tool" provides the following result parameters: Table 3-36 "Turning tool" result parameters Parameter Description Unit _OVR[8] Length actual value L1 mm _OVR[9] Length difference L1 mm _OVR[10] Length actual value L2 mm _OVR[11] Length difference L2 mm _OVR[12] Length actual value L3 mm _OVR[13] Length difference L3 mm 242 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

241 3.4 Measure tool (turning) Parameter Description Unit _OVR[27] Work offset range mm _OVR[28] Safe area mm _OVR[29] Permissible dimensional difference mm _OVR[30] Empirical value mm _OVI[0] D number - _OVI[2] Measuring cycle number - _OVI[3] Measuring version - _OVI[5] Probe number - _OVI[7] Empirical value memory number - _OVI[8] Tool number - _OVI[9] Alarm number Milling tool (CYCLE982) Function This measuring version can be used to measure a milling tool on a turning machine (lathe). The following measurements can be performed: Length Radius Length and radius The measuring cycle checks whether the difference to be corrected with respect to the old tool length or to the old tool radius lies within a defined tolerance range: Upper limits: Safe area TSA and dimensional difference control DIF. Lower limit: Zero offset range TZL. If this range is not violated, the new tool length is accepted in the tool offset, otherwise an alarm is output. Violation of the lower limit is not corrected. The tool length correction is is realized depending on the particular turning machine (lathe). The length assignment (L1 in X, L2 in Y) to the geometry axes is realized just the same as for a turning tool. Measuring principle For a "complete" measurement, all measured variables that can be determined (lengths L1 and L2 and radius) are determined. In both axes (for G18: Z and X) of the plane, probing action is performed with respect to the probe, whereby the measurement starts with the first axis of the plane (for G18: Z). Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 243

242 3.4 Measure tool (turning) For an "axis-by-axis" measurement, the measured variables are measured corresponding to the selection "only length (L1 or L2)", "only radius" or "length (L1 or L2) and radius" only in the parameterized measuring axis of the active plane. Measuring "axis-by-axis" - only length (L1 or L2) Length L1 or L2 is measured in the parameterized measuring axis. Table 3-37 Measuring "axis-by-axis" - only length (L1 or L2) Without milling tool reversal With milling tool reversal Measuring length L2 Measuring length L1 Measuring length L2 Requirement: Radius R must be known. Measuring "axis-by-axis" - only radius The radius in the parameterized measuring axis is measured by probing twice at the probe. Table 3-38 Measuring "axis-by-axis" - only radius Without milling tool reversal With milling tool reversal 244 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

243 3.4 Measure tool (turning) Measuring "axis-by-axis" - only length (L1 or L2) and radius Length L1 or L2 and radius are measured in the parameterized measuring axis by probing twice to two different sides of the measuring probe. Table 3-39 Measuring "axis-by-axis" - only length (L1 or L2) and radius Length L1 and radius measurement without milling tool reversal Length L2 and radius measurement with milling tool reversal Measuring "complete" - lengths (L1 and L2) and radius For complete measurements, all offsets are determined: Both lengths and radius (four measurements). If the radius is specified to be 0, then both lengths are determined (two measurements). The measuring cycle generates the approach blocks to the probe and the transverse motions to measure length 1, length 2 and the radius. A correctly selected start position is required. Milling tool reversal When measuring with reversal, to start, the measuring point in the selected axis and a milling spindle position according to starting angle SPOS is measured. Then the tool (spindle) is turned through 180 degrees and measured again. The average value is the measured value. Measurement with reversal, results in a second measurement at each measuring point with a spindle rotation through 180 degrees with respect to the starting angle. The offset angle entered in SCOR is summed to these 180 degrees. This enables selection of a specific 2nd milling cutting edge that is offset from the 1st cutting edge by precisely 180 degrees. Measurement with reversal permits measurement of two cutting edges of one tool. The mean value is the offset value. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 245

244 3.4 Measure tool (turning) Tool position Axial position Radial position Milling cutter radius in the 2nd measuring axis (for G18: X) Milling cutter radius in the 1st measuring axis (for G18: Z) Measurement with rotating/stationary spindle Measurement is possible with a rotating (M3, M4) or with a stationary milling spindle (M5). If the milling spindle is stationary, at the beginning it is positioned at the specified starting angle SPOS. Note Measurement with rotating spindle If selection of a specific milling tool cutting edge is not possible, it is possible to measure with a rotating spindle. The user must then program the direction of rotation, speed, and feedrate very carefully before calling up CYCLE982 to prevent damage to the probe. A low speed and feedrate must be selected. Empirical values may optionally be included. A mean value is not calculated. Requirements The tool probe must be calibrated, see Calibrate probe (CYCLE982) (Page 234). The approximate tool dimensions must be entered in the tool offset data: Tool type: 1xy (milling tool) Radius, length 1, length 2. The tool to be measured must be active with its tool offset values when the cycle is called. For a milling cutter, the channel-specific SD 42950: $SC_TOOL_LENGTH_TYPE = 2 must be set (length is taken into account just the same as for a turning tool). The tool spindle must be declared as the master spindle. 246 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

245 3.4 Measure tool (turning) Starting position before the measurement From the starting position, collision-free approach to the probe must be possible. The initial positions are located outside the unauthorized area (see the diagram below). 1 to 4 permissible area Image 3-25 Measure milling cutter: Possible starting positions in the 2nd axis of the plane (for G18: X) Position after the end of the measuring cycle For an "axis-by-axis" measurement, the tool tip is positioned at the measurement path distance away from the last probed measuring surface of the probe. For a "complete" measurement, after the measurement, the tool is positioned at the starting point before the cycle was called. Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. tool" softkey. 2. Press the "Milling tool" softkey. The input window "Measure: Milling tool" opens. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 247

246 3.4 Measure tool (turning) Parameter G code program ShopTurn program Parameter Description Unit Parameter Description Unit PL Measuring plane (G17 - G19) - T Name of the tool to be measured Calibration data set (1-6) - D Cutting edge number (1-9) - β Z X Y Calibration data set (1-6) - Tool alignment with swivel axis (0 degrees) (90 degrees) Value entry Start point Z of the measurement Start point X of the measurement Start point Y of the measurement - Degrees mm mm mm Parameters Description Unit Measurement type Axis-by-axis - Complete (measure length and radius) Tool position Axial ( ) - Radial ( ) For measurement type "Complete": Measure Lengths X, Z and radius (in accordance with the tool position) - Cutting edge End face - Rear face Approach Approach probe from the following direction (for measuring plane G18): In the case of tool position "axial": +/- X In the case of tool position "radial": +/- Z - For measurement type "Axis-by-axis": Measure For measuring plane G18: Length X/Z and radius (in accordance with the tool position) Only length Z Only length X Only radius - Milling tool reversal Yes (measurement with reversal of the milling tool (180 )) No (measurement without reversal) Position spindle Set position of the tool spindle (only for milling tool reversal "No") No (any tool spindle position) Yes (position tool spindle at starting angle) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

247 3.4 Measure tool (turning) Parameters Description Unit SPOS Angle for positioning on a tool tip (only for milling cutter reversal "Yes" or position spindle "Yes" or for "complete" measurement type) Degrees SCOR Offset angle for reversal (only for milling tool reversal "Yes") Degrees DFA Measurement path mm TSA Safe area for the measurement result mm TZL Tolerance range for work offset mm TDIF Tolerance range for dimensional difference monitoring mm List of the result parameters The measuring variant "Milling tool" provides the following result parameters: Table 3-40 "Milling tool" result parameters Parameters Description Unit _OVR[8] Length actual value L1 mm _OVR[9] Length difference L1 mm _OVR[10] Length actual value L2 mm _OVR[11] Length difference L2 mm _OVR[12] Radius actual value mm _OVR[13] Radius difference mm _OVR[27] Work offset range mm _OVR[28] Safe area mm _OVR[29] Permissible dimensional difference mm _OVR[30] Empirical value mm _OVI[0] D number - _OVI[2] Measuring cycle number - _OVI[5] Probe number - _OVI[7] Empirical value memory - _OVI[8] Tool number - _OVI[9] Alarm number - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 249

248 3.4 Measure tool (turning) Drill (CYCLE982) Function With this measuring version, the tool length (L1 or L2) of a drill can be measured. The measuring version checks whether the difference to be corrected with respect to the old tool length lies within a defined tolerance range: Upper limits: Safe area TSA and dimensional difference control DIF Lower limit: Zero offset range TZL If this range is not violated, the new tool length is accepted in the tool offset, otherwise an alarm is output. Violation of the lower limit is not corrected. Measuring principle The length (L1 or L2) of the drill is measured in the parameterized measuring axis. Measuring length L2 Measuring length L1 250 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

249 3.4 Measure tool (turning) Tool position: Axial position Radial position Drill radius in the 2nd measuring axis (for G18: X) Drill radius in the 1st measuring axis (for G18: Z) Image 3-26 Measure: drill (CYCLE982), example, tool position: radial position Note If the length of the drill is measured by approaching the probe from the side, then it must be ensured that the drill to be measured does not deflect the probe in the area of the twist groove or in the area of its drill tip. The requirement is that the drill radius was entered in the tool offset, otherwise, an alarm will be output. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 251

250 3.4 Measure tool (turning) Requirements The tool probe must be calibrated. The approximate tool dimensions must be entered in the tool offset data: Tool type: 2xy (drill) Length 1, length 2 The tool to be measured must be active with its tool offset values when the cycle is called. The channel-specific SD 42950: $SC_TOOL_LENGTH_TYPE should be assigned 2 as standard (length assignment the same as for turning tools). For special applications, a value 0 can be used, see Measure drills - special applications (Page 0 ). Starting position before the measurement From the starting position, collision-free approach to the probe must be possible. The initial positions are located outside the unauthorized area (see the diagram below). 1 to 4 permissible area Image 3-27 Measure drill: Possible starting positions in the 2nd axis of the plane (for G18: X) Position after the end of the measuring cycle The tool tip is positioned at the measurement path from the measuring surface. Measure drill - special applications The tool probe has been calibrated with G18 active as is usual for turning tools. Function If drills are used on lathes with a length compensation as for milling machines (SD 42950: $SC_TOOL_LENGTH_TYPE=0), then a drill can also be measured (gauged) in this application. Length L1 is always calculated in the 3rd axis (tool offset axis) of the actual plane G17 to G19. This also characterizes the position of the tool. G17: L1 in Z axis (corresponds to axial position) 252 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

251 3.4 Measure tool (turning) G18: L1 in Y axis (no turning machine application) G19: L1 in X axis (corresponds to radial position) Conditions Length L1 is determined if the following conditions are satisfied: the active tool is of type 2xy (drill) Channel-specific SD 42950: $SC_TOOL_LENGTH_TYPE=0 G17 or G19 are active and Measure drill length L1 for G17 Measure drill length L1 for G19 Procedure The part program or ShopTurn program to be processed has been created and you are in the editor. 1. Press the "Meas. tool" softkey. 2. Press the "Drill" softkey. The input window "Measure: Drill" opens. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 253

252 3.4 Measure tool (turning) Parameters G code program ShopTurn program Parameters Description Unit Parameters Description Unit PL Measuring plane (G17 - G19) - T Name of the tool to be measured Tool position Calibration data set (1-6) - D Cutting edge number (1-9) - Axial ( ) Radial ( ) - Calibration data set (1-6) - β Z X Y Tool alignment with swivel axis (0 degrees) (90 degrees) Value entry Start point Z of the measurement Start point X of the measurement Start point Y of the measurement - Degrees mm mm mm Parameters Description Unit DFA Measurement path mm TSA Safe area for the measurement result mm TZL Tolerance range for work offset mm TDIF Tolerance range for dimensional difference monitoring mm List of the result parameters The measuring variant "Drill" provides the following result parameters: Table 3-41 "Drill" result parameters Parameters Description Unit _OVR[8] Length actual value L1 mm _OVR[9] Length difference L1 mm _OVR[10] Length actual value L2 mm _OVR[11] Length difference L2 mm _OVR[27] Work offset range mm _OVR[28] Safe area mm _OVR[29] Permissible dimensional difference mm _OVR[30] Empirical value mm _OVI[0] D number - _OVI[2] Measuring cycle number - _OVI[3] Measuring version - _OVI[5] Probe number Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

253 3.4 Measure tool (turning) Parameters Description Unit _OVI[7] Empirical value memory - _OVI[8] Tool number - _OVI[9] Alarm number Measure tool with toolholder that can be orientated Overview The functionality is designed for a specific configuration on turning machines (turning/milling machines). As well as the linear axes (Z and X) and main spindle, the turning machines must have swivel axis about Y with accompanying tool spindle. The swivel axis can be used to align the tool on the X/Z level. Preconditions The lateral surfaces of the tool probe should be aligned parallel to the relevant axes (machine or workpiece coordinate system in the 1st and 2nd axis of the plane). The tool probe must be calibrated in the measuring axis and direction in which measuring will be performed. The tool to be measured must be active with its tool offset values when the cycle is called. When measuring turning tools, the cutting edge position of the tool must be entered in the tool offset in accordance with the basic position of the tool carrier. When measuring drilling and milling tools, the setting data must be SD 42950: TOOL_LENGTH_TYPE = 2 i.e., lengths are assigned to the axes in the same way as for turning tools. The active level must be G18. Function To take into account the tool carrier that can be orientated in measuring cycle CYCLE982, the following machine data must be set: MD $MNS_MEA_FUNCTION_MASK, bit 16 = 1 The tool components are corrected corresponding to the orientation of the tool carrier in the initial state. When measuring turning tools, especially roughers, finishers and mushroom-shaped tools, the swivel axis can assume any position around Y. Multiples of 90 are permitted for milling and drilling tools. Multiples of 180 are possible when positioning the tool spindle. This is monitored within the cycle. If turning tools are measured around Y using any positions (not multiples of 90 ) of the swivel axis, then it should be taken into consideration that the turning tool is measured with the same tool position in both axes X/Z, assuming that this is possible. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 255

254 3.4 Measure tool (turning) Sequence Before CYCLE 982 is called, the tool must be aligned in the same way as it will eventually be measured. The tool should be preferably aligned with CYCLE800, refer to the Operating Manual Turning, Chapter "Swivel plane/align tool (CYCLE800)". Please note that the measuring cycle assumes that the tool has been aligned in advance. From the position adopted by the tool, it must be possible to approach the probe in X, Z via the measuring cycle. The measuring procedure that follows is the same as for the measuring variants when the tool carrier is in its basic position. Note Measuring milling tools The following measuring version is not supported when using a tool carrier that can be orientated: Measuring type: "complete" and cutting edge: measure "rear side". When this measuring version is used, alarm 61037: "Incorrect measuring version" is output. 256 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

255 3.5 Measure tool (milling) 3.5 Measure tool (milling) General information The measuring cycles described in this chapter are intended for use on milling machines and machining centers. Note Spindle Spindle commands in the measuring cycles always refer to the active master spindle of the control. When using the measuring cycles at machines with several spindles, then the spindle involved must be defined as master spindle before the cycle call. Reference:/PG/"Programming Guide Fundamentals" Plane definition For milling machines and machining centers, the default setting is the actual machining plane G17. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 257

256 3.5 Measure tool (milling) Machine/workpiece-related measuring/calibrating Machine-related measuring/calibrating: Measuring is performed in the basic coordinate system (machine coordinate system with kinematics transformation disabled). The switching positions of the tool probe refer to the machine zero. Data from the following general setting data are used: SD54625 $SNS_MEA_TP_TRIG_MINUS_DIR_AX1 SD54626 $SNS_MEA_TP_TRIG_PLUS_DIR_AX1 SD54627 $SNS_MEA_TP_TRIG_MINUS_DIR_AX2 SD54628 $SNS_MEA_TP_TRIG_PLUS_DIR_AX2 SD54629 $SNS_MEA_TP_TRIG_MINUS_DIR_AX3 SD54630 $SNS_MEA_TP_TRIG_PLUS_DIR_AX3 Image 3-28 Tool probe, machine-related (G17) Workpiece-related measuring/calibrating: The switching positions of the tool probe refer to the workpiece zero. Data from the following general setting data are used: SD54640 $SNS_MEA_TPW_TRIG_MINUS_DIR_AX1 SD54641 $SNS_MEA_TPW_TRIG_PLUS_DIR_AX1 SD54642 $SNS_MEA_TPW_TRIG_MINUS_DIR_AX2 SD54643 $SNS_MEA_TPW_TRIG_PLUS_DIR_AX2 SD54644 $SNS_MEA_TPW_TRIG_MINUS_DIR_AX3 SD54645 $SNS_MEA_TPW_TRIG_PLUS_DIR_AX3 Image 3-29 Tool probe, workpiece-related (G17) 258 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

257 3.5 Measure tool (milling) Note Workpiece-related or machine-related measurement requires an appropriately calibrated tool probe, see Chapter Calibrate probe (CYCLE971) (Page 259). Compensation strategy The tool measuring cycle is intended for various applications: First measurement of a tool (general setting data SD54762 $SNS_MEA_FUNCTION_MASK_TOOL[Bit9]): The tool offset values in geometry and wear are replaced. The offset is applied in the geometry component of the length or the radius. The wear component is deleted. Post measuring a tool (general setting data SD $SNS_MEA_FUNCTION_MASK_TOOL[Bit9]): The resulting difference is calculated into the wear component (links or radius) of the tool. Empirical values may optionally be included. A mean value is not calculated Calibrate probe (CYCLE971) Function This measuring version calibrates a tool probe machine-related or workpiece-related. Values are corrected without empirical and mean values. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 259

258 3.5 Measure tool (milling) Measuring principle The current clearances between machine zero (machine-related calibration) or workpiece zero (workpiece-related calibration) and the probe trigger point are determined with the aid of the calibration tool. The cycle positions the calibration tool to the probe. Calibrate: Probe (CYCLE971), axis-by-axis Calibrate: Probe (CYCLE971), complete Axis-by-axis calibration For "axis-by-axis" calibration, the probe is calibrated in the parameterized measuring axis and measuring direction. The probing point can be centered in the offset axis. The actual center of the tool probe is determined first in the offset axis before the calibration is performed in the measuring axis General SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX2 General SD $SNS_MEA_TP_TRIG_PLUS_DIR_AX1 General SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX1 Image 3-30 Calibrate probe (CYCLE971) with offset axis, example G17: Determine center in X, calibrate in Y 260 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

259 3.5 Measure tool (milling) Complete calibration The tool probes are automatically calibrated for the "complete" calibration. Using the calibration tool, the measuring cycle determines the tool probe trigger points in all axes or axis directions in which the probe can be approached. See, Commissioning Manual SINUMERIK Operate (IM9) / SINUMERIK 840D sl, Chapter "Tool measurement in milling": General setting data SD $SNS_MEA_TP_AX_DIR_AUTO_CAL or SD $SNS_MEA_TPW_AX_DIR_AUTO_CAL. The tool axis (for G17: Z) must always be able to be approached in the minus direction. Otherwise no "complete" calibration is possible. Calibration is started in the 3rd axis, followed by the axes of the plane. "Complete" calibration is shown in the following screens (example: G17). Image 3-31 Tool probe, disk and cube version Before the first calibration operation in the plane, e.g. plus direction of the 1st axis, the precise center of the probe is determined in the other axis (2nd axis), as long as the probe can be approached in this axis. Additional movements are performed in the plane for this purpose General SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX1 General SD $SNS_MEA_TP_TRIG_PLUS_DIR_AX1 General SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX2 General SD $SNS_MEA_TP_TRIG_PLUS_DIR_AX2 General SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX3 General SD $SNS_MEA_TP_TRIG_PLUS_DIR_AX3 Image 3-32 Determining the probe center in the 2nd axis of the plane, calibration +X Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 261

260 3.5 Measure tool (milling) Requirements The exact length and radius of the calibration tool must be stored in a tool offset data record. This tool offset must be active when the measuring cycle is called. Tool type: Calibration tool (type 725) Milling tool (type 1xy) The machining plane G17 or G18 or G19 must be defined prior to the cycle call. The approximate coordinates of the tool probe must be entered in the general setting data before calibration starts (see Commissioning Manual SINUMERIK Operate (IM9) / SINUMERIK 840D sl, Chapter "Tool measurement in milling"). These values are used for automatic approach to the probe with the calibration tool and their absolute value must not deviate from the actual value by more than the value in parameter TSA. The probe must be reached within the total path 2 x DFA. Starting position before the measurement For "axis-by-axis" calibration, from the starting position, the cycle calculates the approach distance to the probe and generates the appropriate traversing blocks. It must be ensured that a collision-free approach is possible General SD $SNS_MEA_TP_TRIG_PLUS_DIR_AX1 General SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX1 Image 3-33 Starting positions for calibration in the plane, example: G17 Note Calibrating in the 3rd axis of the measuring plane If the tool diameter is larger, the calibration tool is positioned, offset by the tool radius, to the center of the probe. The value of the offset is subtracted. For "complete" calibration, the position before the cycle call should be selected so that a collision-free, centered approach is possible above the probe center by measuring path DFA. 262 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

261 3.5 Measure tool (milling) The axis sequence for the approach is first the tool axis (3rd axis) followed by the axes of the plane. Position after the end of the measuring cycle For "axis-by-axis" calibration, the calibration tool is positioned above the measuring surface by measuring path DFA. For "complete" calibration, the calibration tool is positioned about the center of the probe by measuring path DFA. Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Meas. tool" softkey. 2. Press the "Calibrate probe" softkey. The input window "Calibrate: Probe" opens. Parameters G code program ShopMill program Parameter Description Unit Parameter Description Unit PL Measuring plane (G17 - G19) - T Name of the calibration tool - F Calibration data record (1-6) - D Cutting edge number (1-9) - Calibration and measuring feedrate Distance/ min F Calibration data record (1-6) - Calibration and measuring feedrate mm/min Parameter Description Unit Measurement type Axis-by-axis calibration - Complete calibration Only for measuring mode "axis-by-axis" (for G17): Measuring axis X Y Z - Center probing point No No In Y In X See tool offset - Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 263

262 3.5 Measure tool (milling) Parameter Description Unit Tool offset Direction of the tool offset axis for large tools No Calibration in the 3rd axis: Calibration is performed, centered about the probe. Calibration in the plane: The precise probe center is not defined in the other axis to the measuring axis. In X Calibration in the plane: Prior to the calibration in Y, the precise probe center in X is determined. Calibration in the 3rd axis: See offset In Y Calibration in the plane: Prior to the calibration in X, the precise probe center in Y is determined. Calibration in the 3rd axis: See offset Spindle reversal Compensation of eccentricity through spindle reversal 1) Yes No V Lateral offset (only for measuring axis "Z", for G17) The offset is active when calibrating the 3rd measuring axis, if the calibration tool diameter is larger than the upper diameter of the probe. Here, the tool is offset from the center of the probe by the tool radius, minus the value of V. An offset axis must be specified. DFA Measurement path mm TSA Safe area for the measurement result mm 1) The "Spindle reversal" function is shown if bit 11 is set in the general SD $SNS_MEA_FUNCTION_MASK_TOOL. - - mm List of the result parameters The measuring variant "Calibrate probe" provides the following result parameters: Table 3-42 "Calibrate probe" result parameters Parameters Description Unit _OVR [8] Trigger point in minus direction, actual value of 1st geometry axis mm _OVR [10] Trigger point in plus direction, actual value of 1st geometry axis mm _OVR [12] Trigger point in minus direction, actual value of 2nd geometry axis mm _OVR [14] Trigger point in plus direction, actual value of 2nd geometry axis mm _OVR [16] Trigger point in minus direction, actual value of 3rd geometry axis mm _OVR [18] Trigger point in plus direction, actual value of 3rd geometry axis mm _OVR [9] Trigger point in minus direction, difference of 1st geometry axis mm _OVR [11] Trigger point in plus direction, difference of 1st geometry axis mm _OVR [13] Trigger point in minus direction, difference of 2nd geometry axis mm _OVR [15] Trigger point in plus direction, difference of 2nd geometry axis mm _OVR [17] Trigger point in minus direction, difference of 3rd geometry axis mm _OVR [19] Trigger point in plus direction, difference of 3rd geometry axis mm _OVR [27] Work offset range mm 264 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

263 3.5 Measure tool (milling) Parameters Description Unit _OVR [28] Safe area mm _OVI [2] Measuring cycle number - _OVI [3] Measuring version _OVI [5] Probe number - _OVI [9] Alarm number Milling tool (CYCLE971) Function With this measuring version, the tool length or the tool radius of milling tools can be measured. With milling tools, optionally the cutting edge length or the cutting edge radius can be measured (e.g. to check whether individual cutting edges of the milling tool have been broken out), see Section, Cutting tooth breakage monitoring. A check is made whether the difference to be corrected in the entered tool length or to the entered tool radius in the tool management lies within a defined tolerance range: Upper limit: Safe area TSA and dimensional difference control DIF Lower limit: Work offset range TZL When this area is maintained, the measured tool length or the tool radius is entered in the tool management, otherwise a message is output. Violation of the lower limit is not corrected. Measuring is possible either with: Stationary spindle (see Section Tool measurement with stationary spindle (Page 268)) Rotating spindle (see Section Tool measurement with rotating spindle (Page 268)) Note The cutting tooth breakage monitoring is only possible in conjunction with the "Tool measurement with rotating spindle" function! Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 265

264 3.5 Measure tool (milling) Measuring principle Measure: Milling tool (CYCLE971), example, length Measure: Milling tool (CYCLE971), example, radius The milling tool must always be aligned perpendicular to the probe before the measuring cycle is called, i.e. the tool axis is parallel to the center line of the probe. Image 3-34 Parallel alignment of tool axis, probe axis and axis of the coordinate system Length measurement If the tool diameter is less than the upper diameter of the probe, then the tool is always positioned at the center of the probe. If the tool diameter is larger, the tool is positioned offset by the tool radius toward the center onto the probe. The value of the offset is subtracted. If no offset axis is specified, if necessary an offset is realized in the 1st axis of the plane (with G17: X axis). 266 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

265 3.5 Measure tool (milling) Image 3-35 Length measurement with and without offset Radius measurement The tool radius is measured using lateral probing at the probe in the parameterized measuring axis and measuring direction (see the following diagram). Image 3-36 Radius measurement with and without offset Requirements Note The tool probe must be calibrated before the tool measurement (see Calibrate probe (CYCLE971) (Page 259)). The tool geometry data (approximate values) must be entered in a tool offset data record. The tool must be active. The machining plane must be programmed in which the probe was calibrated. The tool must be prepositioned in such a way that collision-free approach with the probe is possible in the measuring cycle. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 267

266 3.5 Measure tool (milling) Starting position before the measurement Before the cycle call, a starting position must be assumed from which the probe can be approached collision-free. The measuring cycle calculates the direction of approach and generates the appropriate traversing blocks General SD $SNS_MEA_TP_TRIG_PLUS_DIR_AX1 General SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX1 Image 3-37 Calibrate probe (CYCLE971), starting positions for calibration in the plane Position after the end of the measuring cycle The tool is positioned at the measurement path distance away from the measuring surface Measurement with stationary spindle Tool measurement with stationary spindle When measuring milling tools, before the measuring cycle is called, the tool with the spindle must be rotated so that the selected cutting edge can be measured (length or radius) Measurement with rotating spindle Tool measurement with rotating spindle Typically, measurements of the radius of milling tools are executed with rotating spindle, which means that the largest cutting edge determines the measuring result. Likewise, it can make sense to measure the length of milling tools with the spindle rotating. The following must be taken into account: Is it permissible to use the tool probe to perform measurements with rotating spindle with length and/or radius calculation? (manufacturer data) Permissible peripheral (circumferential) speed for the tool to be measured Maximum permissible speed 268 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

267 3.5 Measure tool (milling) Maximum permissible feedrate when probing Minimum feedrate when probing Selecting the direction of rotation depending on the cutting edge geometry to avoid a hard impact when probing at the probe Specified measuring accuracy When performing a measurement with rotating tool, the ratio between the measuring feedrate and speed must be taken into account. In this case, a cutting edge is considered. For multiple cutting edges, the longest cutting edge is responsible for the measuring result. The following interrelationships have to be taken into account: n = S / (2π r 0.001) F = n Δ Where: Metric Basic system Inch n Speed rev/min rev/min S Max. permissible peripheral speed m/min Feet/min r Tool radius mm Inch F Measuring feedrate mm/min inch/min Δ Measuring accuracy mm Inch Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 269

268 3.5 Measure tool (milling) Special issues when performing measurements with rotating spindle As standard, the feedrate and speed with the limit values defined in the general setting data SD SD for peripheral speed, speed, minimum feedrate maximum feedrate and measuring accuracy, as well as the intended direction of spindle rotation for measurement are calculated in a cycle (see Commissioning Manual SINUMERIK Operate (IM9) / SINUMERIK 840D sl, Chapter "Tool measurement in milling - monitoring for measuring with rotating spindle") Measuring is conducted by probing twice; the 1st probing action causes a higher feedrate. A maximum of three probing operations are possible for measuring. If probing is performed several times the speed is additionally reduced on the last probing operation. By setting the general SD $SNS_MEA_FUNCTION_MASK[Bit19], this speed reduction can be suppressed. Using the general SD $SNS_MEA_FUNCTION_MASK_TOOL[Bit5], the user can hide the cycle-internal calculation and enter the values for feedrate and speed via the input screen form of the cycle. To specify the values with bit 5 set in the general SD $SNS_MEA_FUNCTION_MASK_TOOL, the input fields in the screen form F1 (feedrate 1) and S1 (speed 1), F2 (feedrate 2) and S2 (speed 2) or F3 (feed 3) and S3 (Speed 3) are used. For the first probing, the values of F1 and S1 are effective, and for the second probing the values F2 and S2. If S2=0, only one probing action is performed. If S3>0 and S2>0, triple probing is performed, whereby for the 3rd probing, the values from F3 and S3 are effective. The monitoring functions for the general setting data SD SD are not active! If, when calling the measuring cycle, the spindle is stationary, then the direction of rotation is determined from the general SD $SNS_MEA_CM_SPIND_ROT_DIR. Note If, when calling a measuring cycle, the spindle is already rotating, then this direction of rotation is kept independent of the general SD $SNS_MEA_CM_SPIND_ROT_DIR! Cutting tooth breakage monitoring Cutting tooth breakage monitoring The cutting tooth breakage monitoring can be used for remeasuring (offset in the wear) and initial measuring (offset in the geometry). Milling tools with up to 100 cutting edges can be measured. A check is made as to whether the measured values of all cutting edges are within a defined tolerance range: Upper limit: Safe area TSA and dimensional difference control DIF Lower limit: Work offset range TZL If the measured values are outside the tolerance range, an alarm is output. 270 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

269 3.5 Measure tool (milling) If the measured value of the longest cutting edge is within the tolerance range, this is entered in the tool management. Violation of the lower limit is not corrected. Note The cutting tooth breakage monitoring is only possible in conjunction with the Tool measurement with rotating spindle (Page 268) function. Length measurement The tool is positioned to the side of the probe and below the upper edge of the probe in the offset axis. To determine the spindle position of a cutting edge, the probe makes contact twice with the rotating tool. This is followed by the length measurement with stationary spindle. For this purpose, the tool is positioned above the probe and offset by the tool radius to the center of the probe. First, the cutting edge whose spindle position has been determined through lateral contact is measured. The other cutting edges are measured through spindle orientation. After the measurements, the measured value of the longest cutting edge is entered in the tool offset, when this is within the tolerance range. Radius measurement For radius measurement, the distance between the cutting edges must be identical (example: A tool with three cutting edges has a cutting edge every 120 degrees). The tool is positioned to the side of the probe and below the upper edge of the probe in the offset axis. To determine the spindle position of the longest cutting edge, the probe makes contact twice with the rotating tool. The exact spindle position and the cutting edge radius at the highest point of the cutting edge are then measured through multiple contacts when the spindle is stationary. The other cutting edges are measured by changing the spindle orientation. The measured radius of the longest cutting edge is entered in the tool offset, when the value is within the tolerance range. Special issues relating to the cutting tooth breakage monitoring The following additional requirements apply: The number of cutting edges of the milling tool must be entered in the tool offset. Tool spindle with position measuring system. The tool probe must be calibrated, see Calibrate probe (CYCLE971) (Page 259) Before the cycle call, the tool must be positioned next to the probe and above the probe edge. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 271

270 3.5 Measure tool (milling) Image 3-38 Measuring cutting tooth breakage monitoring (CYCLE971), starting position before measuring cycle call Calling the measuring version Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Measure tool" softkey in the vertical softkey bar. 2. Press the "Milling tool" softkey in the horizontal softkey bar. The input window "Measure: Tool" opens Parameters Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit PL Measuring plane (G17 - G19) - T Name of the tool to be measured Calibration data record (1-6) - D Cutting edge number (1-9) - Calibration data record (1-6) - - Parameter Description Unit Measuring Length (measure tool length) - Radius (measure tool radius) Spindle Behavior of spindle during measurement: Spindle stationary Spindle rotates Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

271 3.5 Measure tool (milling) Parameter Description Unit Single cut. edge meas. Cutting tooth breakage monitoring (only with "rotating spindle") 1) Yes No Only for measure "Radius": - Measuring axis Corresponding to the set measuring plane: X (for G17) Y (for G17) DZ Length offset (for G17) mm Only for measure "Length": - Tool offset Offset axis No: The tool is measured,centered. In X In Y V Lateral offset (only for tool offset in X / Y) mm DFA Measurement path mm TSA Safe area for the measurement result mm 1) The "Cutting tooth breakage monitoring" function is shown if bit 10 is set in the general SD $SNS_MEA_FUNCTIONS_MASK_TOOL Result parameters List of the result parameters The measuring version "Milling tool" provides the following result parameters: Table 3-43 "Measure tool" result parameters Parameter Description Unit _OVR [8] Actual value of length L1 1) / length of the longest cutting edge 3) mm _OVR [9] _OVR [10] _OVR [11] Difference of length L1 1) / difference of length of the longest cutting edge 3) Actual value of radius R 2), / actual value of radius of the longest cutting edge 4) Difference of radius R 2) / difference of radius of the longest cutting edge 4) _OVR [12] Actual value of length of the shortest cutting edge 3) mm _OVR [13] Difference of length of the shortest cutting edge 3) mm _OVR [14] Actual value of radius of the shortest cutting edge 4) mm _OVR [15] Difference of radius of the shortest cutting edge 4) mm _OVR [27] Work offset range mm _OVR [28] Safe area mm _OVR [29] Permissible dimensional difference mm _OVR [30] Empirical value mm mm mm mm Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 273

272 3.5 Measure tool (milling) Parameter Description Unit _OVR [100] - _OVR [199] _OVR [200] - _OVR [299] _OVR [300] - _OVR [399] _OVR [400] - _OVR [499] Actual values of the individual radii 4), Difference of the individual radii 4), Actual value of the individual lengths 3) Difference of the individual lengths 3) _OVI [0] D number - _OVI [2] Measuring cycle number - _OVI [3] Measuring version - _OVI [5] Probe number - _OVI [7] Number of the empirical value memory - _OVI [8] T name - _OVI [9] Alarm number - 1) Only for measure "Length" 2) Only for measure "Radius" 3) Only for the "cutting tooth breakage monitoring" function, measure cutting edge length 4) Only for the "cutting tooth breakage monitoring" function, measure cutting edge radius mm mm mm mm Measuring the tool on machines with combined technologies General information This chapter refers to measuring a tool on milling/turning machines. Turning is set up as the 1st technology and milling as the 2nd technology. Preconditions: 1. Milling: MD $MCS_TECHNOLOGY = 2 2. Turning: MD $MCS_TECHNOLOGY_EXTENSION = 1 Further, the following setting data must be set: SD $SC_TOOL_LENGTH_TYPE = 3 SD $SC_TOOL_LENGTH_CONST = 17 SD $SC_TOOL_LENGTH_CONST_T = 19 Additional settings/notes relating to milling/turning technology should be taken from IM9, Chapter "Turning on milling machines". 274 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

273 3.5 Measure tool (milling) Function Using measuring cycles, the probe can be calibrated on milling/turning machines and milling, drilling and turning tools can be measured. A probe is calibrated using the CYCLE971 cycle Cycle CYCLE971 is used to measure milling and drilling tools Cycle CYCLE982 is used to measure turning tools The descriptions for the appropriate cycles in this manual should be used to parameterize the individual measuring versions Drill (CYCLE971) Function With this measuring version, the tool length or the tool radius of drilling tools can be measured. A check is made whether the difference to be corrected in the entered tool length or to the entered tool radius in the tool management lies within a defined tolerance range: Upper limit: Safe area TSA and dimensional difference control DIF Lower limit: Work offset range TZL When this area is maintained, the measured tool length or the tool radius is entered in the tool management, otherwise a message is output. Violation of the lower limit is not corrected. Measuring is possible either with: Stationary spindle (see Section Tool measurement with stationary spindle (Page 268)) Rotating spindle (see Section Tool measurement with rotating spindle (Page 268)) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 275

274 3.5 Measure tool (milling) Measuring principle Measure: Drilling tool (CYCLE971), example, length Measure: Drilling tool (CYCLE971), example, radius The drilling tool must always be aligned perpendicular to the probe before the measuring cycle is called, i.e. the tool axis is parallel to the center line of the probe. Image 3-39 Parallel alignment of tool axis, probe axis and axis of the coordinate system Length measurement If the tool diameter is less than the upper diameter of the probe, then the tool is always positioned at the center of the probe. if the tool diameter is larger, the tool is positioned offset by the tool radius toward the center onto the probe. The value of the offset is subtracted. If no offset axis is specified, if necessary an offset is realized in the 1st axis of the plane (with G17: X axis). 276 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

275 3.5 Measure tool (milling) Image 3-40 Length measurement with and without offset Radius measurement The tool radius is measured using lateral probing at the probe in the parameterized measuring axis and measuring direction (see the following diagram). Image 3-41 Radius measurement with and without offset Preconditions Note The tool probe must be calibrated before the tool measurement (see Calibrate probe (CYCLE971) (Page 259)). The tool geometry data (approximate values) must be entered in a tool offset data record. The tool must be active. The machining plane must be programmed in which the probe was calibrated. The tool must be prepositioned in such as way that collision-free approach with the probe is possible in the measuring cycle. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 277

276 3.5 Measure tool (milling) Starting position before the measurement Before the cycle call, a starting position must be assumed from which the probe can be approached collision-free. The measuring cycle calculates the direction of approach and generates the appropriate traversing blocks General SD $SNS_MEA_TP_TRIG_PLUS_DIR_AX1 General SD $SNS_MEA_TP_TRIG_MINUS_DIR_AX1 Image 3-42 Calibrate probe (CYCLE971), starting positions for calibration in the plane Position after the end of the measuring cycle The tool is positioned at the measurement path distance away from the measuring surface Calling the measuring version Procedure The part program or ShopMill program to be processed has been created and you are in the editor. 1. Press the "Measure tool" softkey in the vertical softkey bar. 2. Press the "Drilling tool" softkey in the horizontal softkey bar. The input window "Measure: Tool" opens. 278 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

277 3.5 Measure tool (milling) Parameters Parameter G code program ShopMill program Parameter Description Unit Parameter Description Unit PL Measuring plane (G17 - G19) - T Name of the tool to be measured Calibration data record (1-6) - D Cutting edge number (1-9) - Calibration data record (1-6) - - Parameter Description Unit Measuring Length (measure tool length) Spindle Radius (measure tool radius) Behavior of spindle during measurement: Spindle stationary Spindle rotates Single cut. edge meas. Cutting tooth breakage monitoring (only with "rotating spindle") 1) Yes No Only for measure "Radius": - Measuring axis Corresponding to the set measuring plane: X (for G17) Y (for G17) DZ Length offset (for G17) mm Only for measure "Length": - Tool offset Offset axis No: The tool is measured,centered. In X In Y V Lateral offset (only for tool offset in X / Y) mm DFA Measurement path mm TSA Safe area for the measurement result mm 1) The "Cutting tooth breakage monitoring" function is shown if bit 10 is set in the general SD $SNS_MEA_FUNCTIONS_MASK_TOOL Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 279

278 3.5 Measure tool (milling) Result parameters List of the result parameters The measuring version "Measure drill" provides the following result parameters: Table 3-44 "Measure tool" result parameters Parameter Description Unit _OVR [8] Actual value of length L1 1) / length of the longest cutting edge 3) mm _OVR [9] _OVR [10] _OVR [11] Difference of length L1 1) / difference of length of the longest cutting edge 3) Actual value of radius R 2), / actual value of radius of the longest cutting edge 4) Difference of radius R 2) / difference of radius of the longest cutting edge 4) _OVR [12] Actual value of length of the shortest cutting edge 3) mm _OVR [13] Difference of length of the shortest cutting edge 3) mm _OVR [14] Actual value of radius of the shortest cutting edge 4) mm _OVR [15] Difference of radius of the shortest cutting edge 4) mm _OVR [27] Work offset range mm _OVR [28] Safe area mm _OVR [29] Permissible dimensional difference mm _OVR [30] Empirical value mm _OVR [100] - _OVR [199] _OVR [200] - _OVR [299] _OVR [300] - _OVR [399] _OVR [400] - _OVR [499] Actual values of the individual radii 4), Difference of the individual radii 4), Actual value of the individual lengths 3) Difference of the individual lengths 3) _OVI [0] D number - _OVI [2] Measuring cycle number - _OVI [3] Measuring version - _OVI [5] Probe number - _OVI [7] Number of the empirical value memory - _OVI [8] T name - _OVI [9] Alarm number - 1) Only for measure "Length" 2) Only for measure "Radius" 3) Only for the "cutting tooth breakage monitoring" function, measure cutting edge length 4) Only for the "cutting tooth breakage monitoring" function, measure cutting edge radius mm mm mm mm mm mm mm 280 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

279 Parameter lists Overview of measuring cycle parameters CYCLE973 measuring cycle parameters PROC CYCLE973(INT S_MVAR,INT S_PRNUM,INT S_CALNUM,REAL S_SETV,INT S_MA,INT S_MD,REAL S_FA,REAL S_TSA,REAL S_VMS,INT S_NMSP,INT S_MCBIT,INT _DMODE,INT _AMODE) Table 4-1 CYCLE973 call parameters 1) No. Screen form parameters Meaning 1 S_MVAR Measuring variant (default= ) Cycle parameters Values: UNITS: Calibration on a surface, edge or in a groove 0 = Length on surface/edge (in the WCS) with known setpoint 1 = Radius on surface (in the WCS) with known setpoint 2 = Length in groove (in the WCS), see S_CALNUM 3 = Radius in groove (in the WCS), see S_CALNUM TENS: Reserved 0 = 0 HUNDREDS: Reserved 0 = 0 THOUSANDS: Selection of measuring axis and measuring direction for calibration 2) 0 = No specification (for surface calibration on the groove base, no selection of the measuring axis and measuring direction) 4) 1 = Specify selection of measuring axis and measuring direction, see S_MA, S_MD (one measuring direction in a measuring axis) 2 = Specify selection of measuring axis, see S_MA (two measuring directions in a measuring axis) TEN THOUSANDS: Determination of the positional deviation (probe skew) 0 = Determine positional deviation 1 = Do not determine positional deviation HUNDRED THOUSANDS: Reserved 0 = 0 ONE MILLION:adapt tool length 7) 0 = Do not adapt tool length (only trigger points) 1 = Adapt tool length 2), 3) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 281

280 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters 2 Icon+ number S_PRNUM Meaning Number of the field of the probe parameters (not probe number) (default=1) 3 S_CALNUM Number of the calibration groove for calibration on a groove (default=1) 5) 4 S_SETV Setpoint for calibration on a surface 5 X0 S_MA Measuring axis (number of the axis) 6) (default=1) 1 = 1st axis of the plane (for G18 Z) 2 = 2nd axis of the plane (for G18 X) 3 = 3rd axis of the plane (for G18 Y) 6) 6 +- S_MD Measuring direction (default=1) Cycle parameters Values: Values: 7 DFA S_FA Measurement path 8 TSA S_TSA Safe area 0 = Positive measuring direction 1 = Negative measuring direction 9 VMS S_VMS Variable measuring velocity for calibration 2) S_NMSP 11 S_MCBIT Reserved 12 _DMODE Display mode Number of measurements at the same location 2) (default=1) 10 Measurements Values: 13 _AMODE Alternative mode 1) All default values = 0 or marked as default=x UNITS: Machining plane G17/G18/G19 0 = compatibility, the plane active before the cycle call remains active 1 = G17 (only active in the cycle) 2 = G18 (only active in the cycle) 3 = G19 (only active in the cycle) 2) Display depends on the general SD $SNS_MEA_FUNCTION_MASK_PIECE 3) Only relevant for calibration in two axis directions 4) Only measuring axis and measuring direction are determined automatically from the cutting edge position (SL) of the probe. SL=8 -X, SL=7 -Z 5) The number of the calibration groove (n) refers to the following general setting data (all positions in machine coordinate system): For cutting edge SL=7: SD54615 $SNS_MEA_CAL_EDGE_BASE_AX1[n] Position of the base of the groove in the 1st axis of the plane (for G18 Z) SD54621 $SNS_MEA_CAL_EDGE_PLUS_DIR_AX2[n] Position of the groove wall in the positive direction of the 2nd axis of the plane (for G18 X) SD54622 $SNS_MEA_CAL_EDGE_MINUS_DIR_AX2[n] Position of the groove wall in the negative direction of the 2nd axis of the plane For cutting edge SL=8: SD54619 $SNS_MEA_CAL_EDGE_BASE_AX2[n] Position of the base of the groove in the 2nd axis of the plane SD54620 $SNS_MEA_CAL_EDGE_UPPER_AX2[n] Position of the upper edge of the groove in the 2nd axis of the plane, (only to pre-position the probe) SD54617 $SNS_MEA_CAL_EDGE_PLUS_DIR_AX1[n] Position of the groove wall in the positive direction of the 1st axis of the plane SD54618 $SNS_MEA_CAL_EDGE_MINUS_DIR_AX1[n] Position of the groove wall in the negative direction of the 1st axis of the plane Note: The position values for the groove wall +- can be roughly determined. 282 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

281 Parameter lists 4.1 Overview of measuring cycle parameters The groove width from the difference of the position values of the groove wall must be able to be precisely determined (precision dial gauge). When calibrating in the groove, it is assumed that the tool length of the probe of the calibrated axis = 0. The position values for the groove base must also be precisely determined at the machine (not just a dimension taken from a drawing). 6) Measuring axis S_MA=3 for calibration on a surface and on a turning machine with real 3rd axis of the plane (for G18 Y). 7) Adapt tool length when calibrating length in the groove, or for lengths at the surface. Workpiece probe in lathes can be defined using 2 lengths (X Z). Turning probe, type 580 cutting-edge position 7: For length calibration, optionally, the Z length is corrected. Turning probe, type 580 cutting edge position 8: For length calibration, optionally, the X length is corrected The tool length is not adapted for the measurement version, radius at groove or radius at the surface. Only the corresponding trigger points are saved CYCLE974 measuring cycle parameters PROC CYCLE974(INT S_MVAR,INT S_KNUM,INT S_KNUM1,INT S_PRNUM,REAL S_SETV,INT S_MA,REAL S_FA,REAL S_TSA,REAL S_STA1,INT S_NMSP,STRING[32] S_TNAME,INT S_DLNUM,REAL S_TZL,REAL S_TDIF,REAL S_TUL,REAL S_TLL,REAL S_TMV,INT S_K,INT S_EVNUM,INT S_MCBIT,INT _DMODE,INT _AMODE) Table 4-2 CYCLE974 call parameters 1) No. Screen form parameters Meaning 1 S_MVAR Measuring version Cycle parameters Values: UNITS: 0 = Measure front face 1 = Inside measurement 2 = Outside measurement TENS: Reserved HUNDREDS: Correction target 0 = Only measurement (no correction of the WO or no tool offset) 1 = Measurement, determination and correction of the WO (see S_KNUM) 3) 2 = Measurement and tool offset (see S_KNUM1) THOUSANDS: Reserved TEN THOUSANDS: Measurement with or without reversal of the main spindle (workspindle) 0 = Measurement without reversal 1 = Measurement with reversal Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 283

282 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning 2 Selection S_KNUM Correction in the work offset (WO) or basic WO or basic reference 2) Cycle parameters Values: UNITS: TENS: 0 = No correction 1 to max. 99 numbers of the work offset or 1 to max. 16 numbers of the basic offset HUNDREDS: Reserved THOUSANDS: Correction in WO or basic WO or basic reference 0 = Correction of the adjustable WO 1 = Correction of the channel-specific basic WO 2 = Correction of the basic reference 3 = Correction of the global basic WO 9 = Correction of the active WO or for G500, last active channel-specific basic WO 0 = Fine correction 6) 1 = Coarse correction 3 Selection S_KNUM1 Correction in tool offset 4 Icon+ number S_PRNUM TEN THOUSANDS: Coarse or fine correction in the WO, basic WO or basic reference Values: UNITS: TENS: HUNDREDS: 2), 4) 0 = No correction 1 to max. 999 D numbers (cutting edge numbers) for tool offset; for additive and setup offset, see also S_DLNUM THOUSANDS: 0 or unique D number TEN THOUSANDS: 0 or unique D number 1 to max if unique D numbers in MD have been set up HUNDRED THOUSANDS: Tool offset 2) 0 = No specification (offset in tool geometry) 1 = Offset of length L1 2 = Offset of length L2 3 = Offset of length L3 4 = Radius offset ONE MILLION: Tool offset 2) 0 = No specification (offset of the tool length wear) 1 = Tool offset, additive offset (AO) 5) Tool offset value is added to the existing AO 2 = Tool offset, setup offset (SO) 5) SO (new) = SO (old) + AO (old) offset value, AO (new) = 0 3 = Tool offset, setup offset (SO) 5) Tool offset value is added to the existing SO 4 = Tool offset, geometry TEN MILLION: Tool offset 2) 0 = No specification (offset in tool geometry normal (not inverted)) 1 = Offset inverted Number of the field of the probe parameters (not probe number) (default=1) 284 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

283 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning 5 X0 S_SETV Setpoint 6 X S_MA Measuring axis (number of the axis) (default=1) Cycle parameters Values: 7 DFA S_FA Measurement path 8 TSA S_TSA Safe area 1 = 1. axis of the plane (for G18 Z) 2 = 2nd axis of the plane (for G18 X) 3 = 3rd axis of the plane (for G18 Y) 5) 9 α S_STA1 Starting angle for measurement with reversal S_NMSP 11 T S_TNAME Tool name 2) Number of measurements at the same location 2) (default=1) 12 DL S_DLNUM Setup additive offset DL number 5) 13 TZL S_TZL Work offset 2), 4) 14 DIF S_TDIF Dimensional difference check 15 TUL S_TUL Upper tolerance limit (incremental to the setpoint) 4) 16 TLL S_TLL Lower tolerance limit (incremental to the setpoint) 4) 17 TMV S_TMV Offset range for averaging 2) 18 FW S_K Weighting factor for averaging 2) 19 EVN S_EVNUM Number of the empirical mean value memory 20 S_MCBIT Reserved 21 _DMODE Display mode 22 _AMODE Alternative mode 10 Measurements Values: Values: 2), 4) 2), 7) UNITS: Machining plane G17/G18/G19 0 = Compatibility, the plane active before the cycle call remains active 1 = G17 (only active in the cycle) 2 = G18 (only active in the cycle) 3 = G19 (only active in the cycle) UNITS: Dimensional tolerance yes/no 0 = No 1 = Yes 1) All default values = 0 or marked as default=x 2) Display depends on the general SD $SNS_MEA_FUNCTION_MASK_PIECE 3) Correction in WO only possible for measurement without reversal 4) For tool offset in the channel-specific MD TOOL_PARAMETER_DEF_MASK, observe bit0 and bit1 5) Only if the "Setup additive offset" function has been set-up in the general MD $MN_MM_NUM_SUMCORR. In addition, in the general MD $MN_MM_TOOL_MANAGEMENT_MASK, bit8 must be set to 1. 6) If WO "fine" has not been set up in MDs, correction is according to WO "coarse" 7) Empirical averaging only possible for tool offset Value range for empirical mean value memory: 1 to 20 numbers (n) of the empirical value memory, see channel-specific SD $SCS_MEA_EMPIRIC_VALUE[n-1] to numbers (n) of the mean value memory, see channel-specific SD $SCS_MEA_AVERAGE_VALUE[n-1] Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 285

284 Parameter lists 4.1 Overview of measuring cycle parameters CYCLE994 measuring cycle parameters PROC CYCLE994(INT S_MVAR,INT S_KNUM,INT S_KNUM1,INT S_PRNUM,REAL S_SETV,INT S_MA,REAL S_SZA,REAL S_SZO,REAL S_FA,REAL S_TSA,INT S_NMSP,STRING[32] S_TNAME,INT S_DLNUM,REAL S_TZL,REAL S_TDIF,REAL S_TUL,REAL S_TLL,REAL S_TMV,INT S_K,INT S_EVNUM,INT S_MCBIT,INT _DMODE,INT _AMODE) Table 4-3 CYCLE994 call parameters 1) No. Screen form parameters Meaning 1 S_MVAR Measuring version UNITS: Inside or outside measurement (default = 1) 1 = Inside measurement 2 = Outside measurement TENS: Reserved HUNDREDS: Correction target 0 = Only measurement (no correction of the WO or no tool offset) 1 = Measurement and determination and correction of the WO (see S_KNUM) 3) 2 = Measurement and tool offset (see S_KNUM1) THOUSANDS: Protection zone 0 = No consideration of a protection zone 1 = Consideration of a protection zone. Traverse axis, 1st axis of the plane (for G18 Z). Measuring axis, see S_MA. 2 = Consideration of a protection zone. Traverse axis, 2nd axis of the plane (for G18 X). Measuring axis, see S_MA. 3 = Consideration of a protection zone. Traverse axis, 3rd axis of the plane (for G18 Y). Measuring axis, see S_MA. 8) 2 Selection S_KNUM Correction of the work offset (WO) or basic WO or basic reference 2) Cycle parameters Values: Values: UNITS: TENS: 0 = No correction 1 to max. 99 numbers of the work offset or 1 to max. 16 numbers of the basic offset HUNDREDS: Reserved THOUSANDS: Correction of WO or basic or basic reference 0 = Correction of the adjustable WO 1 = Correction of the channel-specific basic WO 2 = Correction of the basic reference 3 = Correction of the global basic WO 9 = Correction of the active WO or for G500 in last active channel-specific basic WO TEN THOUSANDS: Coarse or fine correction in the WO, basic WO or basic reference 0 = Fine correction 6) 1 = Coarse correction 286 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

285 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning 3 Selection S_KNUM1 Correction in tool offset 4 Icon+ number S_PRNUM 5 X0 S_SETV Setpoint UNITS: TENS: HUNDREDS: 2), 4) 0 = No correction 1 to max. 999 D numbers (cutting edge numbers) for tool offset; for additive and setup offset, see also S_DLNUM THOUSANDS: 0 or unique D numbers TEN THOUSANDS: 0 or unique D numbers 1 to max , if unique D numbers in MD have been set up HUNDRED THOUSANDS: Tool offset 2) 0 = No specification (offset tool geometry) 1 = Offset of length L1 2 = Offset of length L2 3 = Offset of length L3 4 = Radius offset ONE MILLION: Tool offset 2) 0 = No specification (offset of the tool length wear) 1 = Tool offset, additive offset (AO) 5) Tool offset value is added to the existing AO 2 = Tool offset, setup offset (SO) 5) SO (new) = SO (old) + AO (old) offset value, AO (new) = 0 3 = Tool offset, setup offset (SO) 5) Tool offset value is added to the existing SO 4 = Tool offset, geometry TEN MILLION: Tool offset 2) 0 = No specification (offset in tool geometry normal, not inverted) 1 = Offset inverted Number of the field of the probe parameters (not probe number) (default=1) 6 X S_MA Number of the measuring axis (default=1) Cycle parameters Values: Values: 1 = 1st axis of the plane (for G18 Z) 2 = 2nd axis of the plane (for G18 X) 3 = 3rd axis of the plane (for G18 Y) 8) 7 X1 S_SZA Length of the protection zone in the measuring axis 8 Y1 S_SZO Length of the protection zone in the traverse axis 9 DFA S_FA Measurement path 10 TSA S_TSA Safe area 11 Measurements S_NMSP 12 T S_TNAME Tool name 2) Number of measurements at the same location 2) (default=1) 13 DL S_DLNUM Setup additive offset DL number 5) 2), 4) 14 TZL S_TZL Work offset 15 DIF S_TDIF Dimensional difference check 2), 4) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 287

286 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning 16 TUL S_TUL Upper tolerance limit (incremental to the setpoint) 4) 17 TLL S_TLL Lower tolerance limit (incremental to the setpoint) 4) 18 TMV S_TMV Offset range for averaging 2) 19 FW S_K Weighting factor for averaging 2) 20 EVN S_EVNUM Number of the empirical value memory 21 S_MCBIT Reserved 22 _DMODE Display mode 23 _AMODE Alternative mode Cycle parameters Values: Values: 1) All default values = 0 or marked as default=x 2), 7) UNITS: Machining plane G17/G18/G19 0 = Compatibility, the plane active before the cycle call remains active 1 = G17 (only active in the cycle) 2 = G18 (only active in the cycle) 3 = G19 (only active in the cycle) UNITS: Dimensional tolerance yes/no 0 = No 1 = Yes 2) Display depends on the general SD $SNS_MEA_FUNCTION_MASK_PIECE 3) Correction in WO only possible for measurement without reversal 4) For tool offset, observe the channel MD TOOL_PARAMETER_DEF_MASK 5) Only if the "Setup additive offset" function has been set-up in the general MD $MN_MM_NUM_SUMCORR. In addition, the general MD $MN_MM_TOOL_MANAGEMENT_MASK, bit8 must be set to 1. 6) If WO "fine" has not been set up in MDs, correction is according to WO "coarse" 7) Empirical averaging only possible for tool offset Value range for empirical mean value memory: 1 to 20 numbers (n) of the empirical value memory, see channel-specific SD $SCS_MEA_EMPIRIC_VALUE[n-1] to numbers (n) of the mean value memory, see channel-specific SD $SCS_MEA_AVERAGE_VALUE[n-1] 8) If Y axis is available on the machine CYCLE976 measuring cycle parameters PROC CYCLE976(INT S_MVAR,INT S_PRNUM,REAL S_SETV,REAL S_SETV0,INT S_MA,INT S_MD,REAL S_FA,REAL S_TSA,REAL S_VMS,REAL S_STA1,INT S_NMSP,INT S_SETV1,INT _DMODE,INT _AMODE) 288 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

287 Parameter lists 4.1 Overview of measuring cycle parameters Table 4-4 CYCLE976 call parameters 1) No. Screen form parameters Meaning 1 S_MVAR Measuring version (default=1000) 2 Icon+ number S_PRNUM Cycle parameters Values: 3 S_SETV Setpoint UNITS: Calibration on surface, calibration sphere or calibration ring 2) 0 = Length on surface with known setpoint 1 = Radius in calibration ring with known diameter (setpoint) and known center point. 2 = Radius in calibration ring with known diameter (setpoint) and an unknown center point 3 = Radius and length at the calibration sphere 4 = Radius at the edge with known setpoint. Note selection of measuring axis and measuring direction. 3) 5 = Radius between two edges with known setpoint and edge clearance. Measuring axis should be selected. TENS: Reserved 0 = 0 HUNDREDS: Reserved 0 = 0 0 = No specification (no selection of the measuring axis and measuring direction required) 8) 1 = Specify selection of measuring axis and measuring direction, see S_MA, S_MD (one measuring direction in a measuring axis) 2 = Specify selection of measuring axis, see S_MA (two measuring directions in a measuring axis) TEN THOUSANDS: Determination of the positional deviation (probe skew) 2) 0 = Determine positional deviation of the probe 6) 1 = Do not determine positional deviation HUNDRED THOUSANDS: Paraxial calibration or at an angle 0 = Paraxial calibration in the active WCS 1 = Calibration at an angle 7) ONE MILLION: Determination of tool length during calibration on surface or on sphere 0 = Do not determine tool length 1 = Determine tool length 4) Number of the field of the probe parameters (not probe number) (default=1) 4 Z0 S_SETV0 Setpoint of the length for sphere calibration 5 X / Y / Z S_MA Measuring axis (number of the axis) 2), 6) (default=1) THOUSANDS: Selection of measuring axis and measuring direction during calibration. Values: 1 = 1. axis of the plane (for G17 X) 2 = 2nd axis of the plane (for G17 Y) 3 = 3rd axis of the plane (for G17 Z) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 289

288 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning S_MD Measuring direction Cycle parameters Values: 2), 6) 0 = Positive 1 = Negative 7 DFA S_FA Measurement path 8 TSA S_TSA Safe area 9 VMS S_VMS Variable measuring velocity for calibration 2) 10 α S_STA1 Starting angle S_NMSP 2), 5) Number of measurements at the same location 2) (default=1) 12 X0 S_SETV1 Edge reference point when calibrating between 2 edges 3) 13 _DMODE Display mode 11 Measurements Values: 14 _AMODE Alternative mode 1) All default values = 0 or marked as default=x UNITS: Machining plane G17/G18/G19 0 = Compatibility, the plane active before the cycle call remains active 1 = G17 (only active in the cycle) 2 = G18 (only active in the cycle) 3 = G19 (only active in the cycle) 2) Display depends on the general SD $SNS_MEA_FUNCTION_MASK_PIECE 3) For "Radius in the calibration ring" calibration, the diameter and the center point of the ring must be known (four measuring directions). For "Radius on two edges" calibration, the distance to the edges in the direction of the measuring axis must be known (two measuring directions). For "Radius on one edge" calibration, the setpoint of the surface must be known. 4) Measuring variant only calibration on a surface (length on surface), corrected tool length results from S_MD and S_MA. 5) Only for measuring variant "Calibration ring,... and known center point" (S_MVAR=1xxx02). 6) Measuring axis only for measuring variant S_MVAR=0 or =xx1x01 or =xx2x01 or =20000 Measuring variant: "Calibration on a surface" selection of measuring axis and measuring direction or on the "Calibration ring,... and known center point" selection of an axis direction and selection of measuring axis and measuring direction or on the "Calibration ring,... and known center point" selection of two axis directions and selection of measuring axis or "Determination of the probe length" S_MA=3 3rd axis of the plane (for G17 Z) 7) Measuring version, only calibration in calibration ring or on calibration sphere For "Calibration on calibration sphere", for measuring at an angle, the axis circles around the sphere at the equator. 8) For "Radius in calibration ring" calibration with unknown center point, four measuring directions in the plane (for G17 +-X +-Y). For "Length on surface" calibration in minus direction of the tool axis (for G17 -Z). 290 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

289 Parameter lists 4.1 Overview of measuring cycle parameters CYCLE978 measuring cycle parameters PROC CYCLE978(INT S_MVAR,INT S_KNUM,INT S_KNUM1,INT S_PRNUM,REAL S_SETV,REAL S_FA,REAL S_TSA,INT S_MA,INT S_MD,INT S_NMSP,STRING[32] S_TNAME,INT S_DLNUM,REAL S_TZL,REAL S_TDIF,REAL S_TUL,REAL S_TLL,REAL S_TMV,INT S_K,INT S_EVNUM,INT S_MCBIT,INT _DMODE,INT _AMODE) Table 4-5 CYCLE978 call parameters 1) No. Screen form parameters Meaning 1 S_MVAR Measuring version Cycle parameters Values: UNITS: Contour element 0 = Measure surface TENS: Reserved HUNDREDS: Correction target 0 = Only measurement (no correction of the WO or no tool offset) 1 = Measurement, determination and correction of the WO (see S_KNUM) 2 = Measurement and tool offset (see S_KNUM1) THOUSANDS: Reserved TEN THOUSANDS: Measurement with/without spindle reversal or align measuring probe in the switching direction 9) 0 = Measurement without spindle reversal, without probe alignment 1 = Measurement with spindle reversal 2 = Align probe in switching direction 2 Selection S_KNUM Correction of the work offset (WO) or basic WO or basic reference 2) Values: UNITS: TENS: 0 = No correction 1 to max. 99 numbers of the work offset or 1 to max. 16 numbers of the basic offset HUNDREDS: Reserved THOUSANDS: Correction of WO or basic or basic reference 0 = Correction of the adjustable WO 1 = Correction of the channel-specific basic WO 2 = Correction of the basic reference 3 = Correction of the global basic WO 9 = Correction of the active WO or for G500 in last active channel-specific basic WO TEN THOUSANDS: Coarse or fine correction in the WO, basic WO or basic reference 0 = Fine correction 6) 1 = Coarse correction Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 291

290 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning 3 Selection S_KNUM1 Correction in tool offset 2) S_PRNUM Cycle parameters Values: 5 X0 S_SETV Setpoint UNITS: TENS: HUNDREDS: 6 DFA S_FA Measurement path 7 TSA S_TSA Safe area 0 = No correction 1 to max. 999 D numbers (cutting edge numbers) for tool offset, for additive and setup offset, see also S_DLNUM THOUSANDS: 0 or unique D numbers TEN THOUSANDS: 0 or unique D numbers 1 to max if unique D numbers in MDs have been set up HUNDRED THOUSANDS: Tool offset 2) 0 = No specification (offset in tool geometry) 1 = Offset of length L1 2 = Offset of length L2 3 = Offset of length L3 4 = Radius offset ONE MILLION: Tool offset 2) 0 = No specification (offset of the tool radius wear) 1 = Tool offset, additive offset (AO) 5) Tool offset value is added to the existing AO 2 = Tool offset, setup offset (SO) 5) SO (new) = SO (old) + AO (old) offset value, AO (new) = 0 3 = Tool offset, setup offset (SO) 5) Tool offset value is added to the existing SO 4 = Tool offset, geometry TEN MILLION: Tool offset 2) 0 = No specification (offset in tool geometry normal, not inverted) 1 = Offset inverted Number of the field of the probe parameter (not probe number) (value range 1 to 12) 8 X S_MA Number of the measuring axis 7) (value range 1 to 3) 9 S_MD Measuring direction of the measuring axis 10 Measurements 4 Icon+number Values: Values: 1 = 1st axis of the plane (for G17 X) 2 = 2nd axis of the plane (for G17 Y) 3 = 3rd axis of the plane (for G17 Z) Measurement in tool direction 1 = Positive measuring direction 2 = Negative measuring direction S_NMSP Number of measurements at the same location 2) (value range 1 to 9) 11 TR S_TNAME Tool name 3) 12 DL S_DLNUM Setup additive offset DL number 5) 13 TZL S_TZL Work offset 14 DIF S_TDIF Dimensional difference check 2), 3) 2), 3) 292 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

291 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning 15 TUL S_TUL Upper tolerance limit (incremental to the setpoint) 3) 16 TLL S_TLL Lower tolerance limit (incremental to the setpoint) 3) 17 TMV S_TMV Offset range for averaging 2) 18 FW S_K Weighting factor for averaging 2) 19 EVN S_EVNUM Date set, empirical value memory 20 S_MCBIT Reserved 21 _DMODE Display mode 22 _AMODE Alternative mode Cycle parameters Values: Values: 2), 8) UNITS: Machining plane G17/G18/G19 0 = Compatibility, the plane active before the cycle call remains active 1 = G17 (only active in the cycle) 2 = G18 (only active in the cycle) 3 = G19 (only active in the cycle) UNITS: Dimensional tolerance yes/no 0 = No 1 = Yes 1) All default values = 0 or marked as the range of values a to b 2) Display depends on the general SD $SNS_MEA_FUNCTION_MASK_PIECE 3) Only for offset in tool, otherwise parameter = "" 4) Only for offset in tool and dimensional tolerance "Yes", otherwise parameter = 0 5) Only if the "Setup additive offset" function has been set-up in the general MD $MN_MM_NUM_SUMCORR. In addition, in the general MD $MN_MM_TOOL_MANAGEMENT_MASK, bit8 must be set to 1. 6) If WO "fine" has not been set up in MDs, correction is according to WO "coarse" 7) Offset in tool geometry: For measurement in the plane (S_MA=1 or S_MA=2) Offset in tool radius For measurement in tool direction (S_MA=3) Offset in tool length L1 8) Empirical averaging for tool offset and correction in WO possible Value range for empirical mean value memory: 1 to 20 numbers (n) of the empirical value memory, see channel-specific SD $SCS_MEA_EMPIRIC_VALUE[n-1] to numbers (n) of the mean value memory, see channel-specific SD $SCS_MEA_AVERAGE_VALUE[n-1] 9) When measuring with spindle reversal, the radius/diameter of the probe must be precisely determined. This should be realized with a calibration version of the CYCLE976 radius at the ring or at the edge or at the sphere. Otherwise, the measurement result will be falsified CYCLE998 measuring cycle parameters PROC CYCLE998(INT S_MVAR,INT S_KNUM,INT S_RA,INT S_PRNUM,REAL S_SETV,REAL S_STA1,REAL S_INCA,REAL S_FA,REAL S_TSA,INT S_MA,INT S_MD,REAL S_ID,REAL S_SETV0,REAL S_SETV1,REAL S_SETV2,REAL S_SETV3,INT S_NMSP,INT S_EVNUM,INT _DMODE,INT _AMODE) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 293

292 Parameter lists 4.1 Overview of measuring cycle parameters Table 4-6 CYCLE998 call parameters 1) No. Screen form parameters Meaning 1 S_MVAR Measuring variant (default=5) UNITS: Contour element 5 = Measure edge (one angle) 6 = Measure plane (two angles) TENS: Reserved HUNDREDS: Correction target 0 = Only measurement and no correction of WO 1 = Measurement, determination and correction of the WO (see S_KNUM) THOUSANDS: Protection zone 0 = No consideration of a protection zone 1 = Consideration of a protection zone TEN THOUSANDS: Measurement with spindle reversal (difference measurement) 0 = Measurement without spindle reversal 1 = Measurement with spindle reversal HUNDRED THOUSANDS: Measurement at an angle or paraxial 0 = Measurement at an angle 1 = Measurement paraxial 2 Selection S_KNUM Correction of the work offset (WO) or basic WO or basic reference 2) 3 A, B, C 4 Icon+ number S_RA S_PRNUM UNITS: TENS: 0 = No correction 1 to max. 99 numbers of the work offset or 1 to max. 16 numbers of the basic offset HUNDREDS: Reserved THOUSANDS: Correction of WO or basic or basic reference 0 = Correction adjustable WO 1 = correction, channel-specific basic WO 2 = correction basic reference 9 = Correction active WO and/or for G500 in last active channel-specific basic WO TEN THOUSANDS: Coarse or fine correction in the WO or basic WO or basic reference 3) 0 = Fine correction 1 = Coarse correction Correction target coordinate rotation or rotary axis Cycle parameters Values: Values: Values: 0 = Correction target coordinate rotation around the axis that results from parameter S_MA 4) >0 = Correction target rotary axis. Number of the channel axis number of the rotary axis (preferably rotary table). The angle offset is made in the translatory part of the WO of the rotary axis. Number of the field of the probe parameter (default=1) 5 DX / DY / DZ S_SETV Distance (incremental) from the starting position to measuring point P1 of the measuring axis (S_MA) 5) 294 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

293 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning 6 α S_STA1 Angle setpoint for "Align edge" or for "Align plane" around the 1st axis of the plane (for G17 X) 9) 7 β S_INCA Angle setpoint for "Align plane" around the 2nd axis of the plane (for G17 Y) 9) 8 DFA S_FA Measurement path 9 TSA S_TSA Safe area Monitoring of the angle difference to the angle setpoint [degrees] 6) 10 X / Y / Z S_MA Measuring axis, offset axis 7) (default=201) UNITS: Number of the measuring axis 1 = 1st axis of the plane (for G17 X) 2 = 2nd axis of the plane (for G17 Y) 3 = 3rd axis of the plane (for G17 Z) TENS: Reserved HUNDREDS: Number of the offset axis 1 = 1st axis of the plane (for G17 X) 2 = 2nd axis of the plane (for G17 Y) 3 = 3rd axis of the plane (for G17 Z) S_MD Measuring direction of the measuring axis 8) Cycle parameters Values: Values: 0 = Measuring direction is determined from the setpoint and the actual position of the measuring axis (compatibility) 1 = Positive measuring direction 2 = Negative measuring direction 12 L2 S_ID For measuring version "Align edge": Distance (incremental) between the measuring points P1 and P2 in the offset axis (value >0) For measuring version "Align plane", the parameters listed below apply. 13 L2 S_SETV0 Distance between the measuring points P1 and P2 in the 1st axis of the plane 10) 14 S_SETV1 Distance between the measuring points P1 and P2 in the 2nd axis of the plane 15 L3x S_SETV2 Distance between the measuring points P1 and P3 in the 1st axis of the plane 11) 16 L3y S_SETV3 Distance between the measuring points P1 and P3 in the 2nd axis of the plane 10) S_NMSP Number of measurements at the same location 2) (default=1) 18 S_EVNUM Date set, empirical value memory 19 _DMODE Display mode 17 Measurements Values: 20 _AMODE Reserved (alternative mode) 1) All default values = 0 or marked as default=x 2), 13) UNITS: Machining plane G17/G18/G19 0 = compatibility, the plane active before the cycle call remains active 1 = G17 (only active in the cycle) 2 = G18 (only active in the cycle) 3 = G19 (only active in the cycle) 2) Display depends on the general SD $SNS_MEA_FUNCTION_MASK_PIECE 3) WO "fine"only if correction target is rotary axis and MD $MCS_AXIS_USAGE_ATTRIB[n] Bit6=1. If WO has not been set up in MDs, correction is according to WO "coarse". 4) Example for offset in coordinate rotation: S_MA=102 Measuring axis Y, offset axis X results in coordinate rotation around Z (for G17) 5) Value only relevant for protection zone "Yes" (S_MVARTHOUSANDS position = 1) 11), 12) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 295

294 Parameter lists 4.1 Overview of measuring cycle parameters 6) When positioning from measuring point P1 to measuring point P2 in the offset axis, the angles in parameters S_STA1 and S_TSA are added. 7) Number of the measuring axis must not be the same as the number of the offset axis (e.g. 101 not permitted) 8) Measuring direction only for "Align edge" and "Measurement paraxial" (S_MVAR=10x105) 9) Angular range S_STA1 ±45 degrees for "Align edge" Angular range S_STA1 0 to +60 degrees and S_INCA ±30 degrees for "Align plane" 10) For measuring versions "Align plane" and "Align edge" 11) For measuring variant "Measure plane" and "Measurement paraxial" 12) Not for measuring cycle version SW ) Experience value generation for correction in WO; value range of empirical values mean value memory: 1 to 20 numbers(n) of the empirical value memory, see channel-specific SD $SCS_MEA_EMPIRIC_VALUE[n-1] CYCLE977 measuring cycle parameters PROC CYCLE977(INT S_MVAR,INT S_KNUM,INT S_KNUM1,INT S_PRNUM,REAL S_SETV,REAL S_SETV0,REAL S_SETV1,REAL S_FA,REAL S_TSA,REAL S_STA1,REAL S_ID,REAL S_SZA,REAL S_SZO,INT S_MA,INT S_NMSP,STRING[32] S_TNAME,INT S_DLNUM,REAL S_TZL,REAL S_TDIF,REAL S_TUL,REAL S_TLL,REAL S_TMV,INT S_K,INT S_EVNUM,INT S_MCBIT,INT _DMODE,INT _AMODE) Table 4-7 CYCLE977 call parameters 1) No. Screen form parameters Meaning 1 S_MVAR Measuring version Cycle parameters Values: UNITS: Contour element (value range 1 to 6) 1 = Measure hole 2 = Measure spigot (shaft) 3 = Measure groove 4 = Measure rib 5 = Measure rectangle, inside 6 = Measure rectangle, outside TENS: Reserved HUNDREDS: Correction target 0 = Only measurement (no correction of the WO or no tool offset) 1 = Measurement, determination and correction of the WO (see S_KNUM) 2 = Measurement and tool offset (see S_KNUM1) THOUSANDS: Protection zone 0 = No consideration of a protection zone 1 = Consideration of a protection zone TEN THOUSANDS: Measurement with/without spindle reversal (differential measurement) or align measuring probe in the switching direction 0 = Measurement without spindle reversal, do not align probe 1 = Measurement with spindle reversal 2 = Align probe in switching direction 296 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

295 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning 2 Selection S_KNUM Correction of the work offset (WO) or basic WO or basic reference 2) Cycle parameters Values: UNITS: TENS: 0 = No correction 1 to max. 99 numbers of the work offset or 1 to max. 16 numbers of the basic offset HUNDREDS: Reserved THOUSANDS: Correction of WO or basic or basic reference 0 = Correction of the adjustable WO 1 = Correction of the channel-specific basic WO 2 = Correction of the basic reference 3 = Correction of the global basic WO 9 = Correction of the active WO or for G500 in last active channel-specific basic WO 0 = Fine correction 6) 1 = Coarse correction 3 Selection S_KNUM1 Correction in tool offset 2) TEN THOUSANDS: Coarse or fine correction in the WO, basic WO or basic reference Values: UNITS: TENS: HUNDREDS: 0 = No correction 1 to max. 999 D numbers (cutting edge numbers) for tool offset; for additive and setup offset, see also S_DLNUM THOUSANDS: 0 or unique D numbers TEN THOUSANDS: 0 or unique D numbers 1 to max if unique D numbers in MDs have been set up HUNDRED THOUSANDS: Tool offset 2) 0 = No specification (offset tool radius) 1 = Offset of length L1 2 = Offset of length L2 3 = Offset of length L3 4 = Radius offset ONE MILLION: Tool offset 2) 0 = No specification (offset of the tool radius wear) 1 = Tool offset, additive offset (AO) 5) Tool offset value is added to the existing AO 2 = Tool offset, setup offset (SO) 5) SO (new) = SO (old) + AO (old) offset value, AO (new) = 0 3 = Tool offset, setup offset (SO) 5) Tool offset value is added to the existing SO 4 = Tool offset, geometry TEN MILLION: Tool offset 2) 0 = No specification (offset in tool geometry normal, not inverted) 1 = Offset inverted Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 297

296 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters 4 Icon+ number S_PRNUM Meaning 5 X0 S_SETV Setpoint Number of the field of the probe parameter (not probe number) (value range 1 to 12) 6 X0 S_SETV0 Setpoint for rectangle in 1st axis of the plane (X for G17) 7 Y0 S_SETV1 Setpoint for rectangle in 2nd axis of the plane (Y for G17) 8 DFA S_FA Measurement path 9 TSA S_TSA Safe area 10 α 0 S_STA1 Starting angle 11 DZ S_ID Absolute incremental value 1. Incremental infeed of the 3rd axis of the plane (Z for G17) Infeed direction via sign of S_ID. For measurement of spigot, rib and rectangle outside, S_ID is used to define the lowering to measuring height. 2. Consideration of a protection zone For measurement of hole, groove and rectangle inside and a protection zone, S_ID is used to define the overtravel height. 12 X1 S_SZA Diameter or length (width) of the protection zone 7) 13 Y1 S_SZO For "Measure rectangle": Width of the protection zone of the 2nd axis of the plane 14 X S_MA Number of the measuring axis 7) (only for measurement of groove or rib) Cycle parameters Values: 1 = 1st axis of the plane (for G17 X) 2 = 2nd axis of the plane (for G17 Y) S_NMSP Number of measurements at the same location 2) (value range 1 to 9) 16 TR S_TNAME Tool name 2) 17 DL S_DLNUM Setup additive offset DL number 5) 2), 4) 18 TZL S_TZL Work offset 19 DIF S_TDIF Dimensional difference check 20 TUL S_TUL Upper tolerance limit (incremental to the setpoint) 4) 21 TLL S_TLL Lower tolerance limit (incremental to the setpoint) 4) 22 TMV S_TMV Offset range for averaging 2) 23 FW S_K Weighting factor for averaging 2) 24 S_EVNUM Data set, empirical mean value memory 25 S_MCBIT Reserved 26 _DMODE Display mode 27 _AMODE Alternative mode 15 Measurements Values: Values: 2), 4) 2), 8) UNITS: Machining plane G17/G18/G19 0 = Compatibility, the plane active before the cycle call remains active 1 = G17 (only active in the cycle) 2 = G18 (only active in the cycle) 3 = G19 (only active in the cycle) UNITS: Dimensional tolerance yes/no 0 = No 1 = Yes 1) All default values = 0 or marked as the range of values a to b 298 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

297 Parameter lists 4.1 Overview of measuring cycle parameters 2) Display depends on the general SD $SNS_MEA_FUNCTION_MASK_PIECE 3) Only for offset in tool, otherwise parameter = "" 4) Only for offset in tool and dimensional tolerance "Yes", otherwise parameter = 0 5) Only if the "Setup additive offset" function has been set-up in the general MD $MN_MM_NUM_SUMCORR. In addition, in the general MD $MN_MM_TOOL_MANAGEMENT_MASK, bit8 must be set to 1. 6) If WO "fine" has not been set up in MDs, correction is according to WO "coarse" 7) Diameter or width of the protection zone within a hole or groove Diameter or width of the protection zone outside of a spigot or rib 8) Empirical averaging possible for tool offset Value range for empirical mean value memory: 1 to 20 numbers (n) of the empirical value memory, see channel-specific SD $SCS_MEA_EMPIRIC_VALUE[n-1] to numbers (n) of the mean value memory, see channel-specific SD $SCS_MEA_AVERAGE_VALUE[n-1] CYCLE961 measuring cycle parameters PROC CYCLE961(INT S_MVAR,INT S_KNUM,INT S_PRNUM,REAL S_SETV0,REAL S_SETV1,REAL S_SETV2,REAL S_SETV3,REAL S_SETV4,REAL S_SETV5,REAL S_SETV6,REAL S_SETV7,REAL S_SETV8,REAL S_SETV9,REAL S_STA1,REAL S_INCA,REAL S_ID,REAL S_FA,REAL S_TSA,INT S_NMSP,INT S_MCBIT,INT _DMODE,INT _AMODE) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 299

298 Parameter lists 4.1 Overview of measuring cycle parameters Table 4-8 CYCLE961 call parameters 1) No. Screen form parameters Meaning 1 S_MVAR Measuring version (default 6) Cycle parameters Values: UNITS: Contour element 5 = Setup of right-angled inside corner, setpoint specification of angle and distances A1 to A3 6 = Setup of right-angled outside corner, setpoint specification of angle and distances A1 to A3 7 = Setup of inside corner, specification of angle and distances A1 to A4 8 = Setup of outside corner, specification of angle and distances A1 to A4 TENS: Setpoint specification as distance or via four points 0 = Setpoint specification as distance (polar) 1 = Setpoint specification using four points (measuring points P1 to P4) HUNDREDS: Correction target 0 = Only measurement (no correction of WO or no tool offset) 1 = Measurement, determination and correction of the WO, see S_KNUM THOUSANDS: Protection zone 0 = No consideration of a protection zone (obstacle) 1 = Consideration of a protection zone (obstacle), see S_ID TEN THOUSANDS: Position of the corner in the WCS 0 = Position of the corner is determined using parameter S_STA1 (compatibility) 1 = Position 1 of the corner at the positioned starting point of the measurement 6) 2= Position 2 of the corner, distances in the 1st axis of the plane (for G17 X) are negative (see S_SETV0, S_SETV1) 3 = Position 3 of the corner, distances in the 1st and 2nd axis of the plane (for G17 XY) are negative (sees_setv0to S_SETV3) 4 = Position 4 of the corner, distances in the 2nd axis of the plane (for G17 Y) are negative (see S_SETV2, S_SETV3) 2 Selection S_KNUM Correction of the work offset (WO) or basic WO or basic reference 2) Values: UNITS: TENS: 0 = No correction 1 to max. 99 numbers of the work offset or 1 to max. 16 numbers of the basic offset HUNDREDS: Reserved THOUSANDS: Correction of WO or basic or basic reference 0 = Correction adjustable WO 1 = correction, channel-specific basic WO 2 = correction basic reference 9 = Correction active WO and/or for G500 last active channel-specific basic WO TEN THOUSANDS: Coarse or fine correction in the WO, basic WO or basic reference 0 = Fine correction 5) 1 = Coarse correction 300 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

299 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters 3 Icon+ number Cycle parameters S_PRNUM Meaning Number of the field of the probe parameter (not probe number) (value range 1 to 12) 4 L1/X1 S_SETV0 Distance L1 between the pole and measuring point P1 in the direction of the 1st axis of the plane (for G17 X) 3) (if the actual distance L1=0, then L1 = M_SETV1 / 2 is automatically calculated) or starting point P1x of the 1st axis of the plane (for G17 X) 4) 5 L2/Y1 S_SETV1 Distance L2 between the pole and measuring point P2 in the direction of the 1st axis of the plane 3) or starting point P1y of the 2nd axis of the plane (for G17 Y) 4) 6 L3/X2 S_SETV2 Distance L3 between the pole and measuring point P3 in the direction of the 2nd axis of the plane 3) (if the distance L3=0, then for a corner that is not right angled, L3 = M_SETV3 / 2 is automatically calculated) or starting point P2x of the 1st axis of the plane 4) 7 L4/Y2 S_SETV3 Distance L4 between the pole and measuring point P3 in the direction of the 2nd axis of the plane with a corner that is not right angled 3) or starting point P2y of the 2nd axis of the plane 4) 8 XP/X3 S_SETV4 Position of the pole in the 1st axis of the plane 3) or starting point P3x of the 1st axis of the plane 4) 9 XP/Y3 S_SETV5 Position of the pole in the 2nd axis of the plane 3) or starting point P3y of the 2nd axis of the plane 4) 10 X4 S_SETV6 Starting point P4x of the 1st axis of the plane 4) 11 Y4 S_SETV7 Starting point P4y of the 2nd axis of the plane 4) 12 X0 S_SETV8 Setpoint of the measured corner in the 1st axis of the plane for correcting in WO 13 Y0 S_SETV9 Setpoint of the measured corner in the 2nd axis of the plane for correcting in WO 14 α0 S_STA1 Starting angle from the positive direction of the 1st axis of the plane to the reference edge of the workpiece in the MCS (+-270 degrees) 15 α1 S_INCA Angle between workpiece reference edges when measuring a non-right-angled corner 7) 16 DZ S_ID Infeed amount at the measuring height for each measuring point for active protection zone (see S_MVAR). 17 DFA S_FA Measurement path 18 TSA S_TSA Safe area Monitoring the angular difference to the angle setpoint [degrees] S_NMSP Number of measurements at the same location 2) (value range 1 to 9) 2) 20 S_MCBIT Reserved 21 _DMODE Display mode 19 Measurements Values: 22 _AMODE Alternative mode UNITS: Machining plane G17/G18/G19 1) All default values = 0 or marked as the range of values a to b 0 = compatibility, the plane active before the cycle call remains active 1 = G17 (only active in the cycle) 2 = G18 (only active in the cycle) 3 = G19 (only active in the cycle) 2) Display depends on the general SD $SNS_MEA_FUNCTION_MASK_PIECE Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 301

300 Parameter lists 4.1 Overview of measuring cycle parameters 3) ) Input of the measuring points in polar coordinates, taking into account the starting angle S_STA1 for measuring point 3 or 4 of the incremental angle S_INCA. 4) Input of the measuring points in the right-angled coordinate system (input using 4 points), 5) If WO "fine" has not been set up in MDs, correction is made according to WO "coarse" 6) Value range of angle S_INCA: -180 to +180 degrees 7) Starting angle S_STA1, value range: right-angled corner: degrees, any corner: degrees CYCLE979 measuring cycle parameters PROC CYCLE979(INT S_MVAR,INT S_KNUM,INT S_KNUM1,INT S_PRNUM,REAL S_SETV,REAL S_FA,REAL S_TSA,REAL S_CPA,REAL S_CPO,REAL S_STA1,REAL S_INCA,INT S_NMSP,STRING[32] S_TNAME,REAL S_DLNUM,REAL S_TZL,REAL S_TDIF,REAL S_TUL,REAL S_TLL,REAL S_TMV,INT S_K,INT S_EVNUM,INT S_MCBIT,INT _DMODE,INT _AMODE) Table 4-9 CYCLE979 call parameters 0) No. Screen form parameters Meaning 1 S_MVAR Measuring version Cycle parameters Values: UNITS: Contour element 1 = Measure hole 2 = Measure spigot (shaft) TENS: Reserved HUNDREDS: Correction target 0 = Only measurement (no correction of the WO or no tool offset) 1 = Measurement, determination and correction of the WO (see S_KNUM) 2 = Measurement and tool offset (see S_KNUM1) THOUSANDS: Number of measurement points 0 = 3 measuring points 1 = 4 measuring points TEN THOUSANDS: Measurement with/without spindle reversal (differential measurement) or align measuring probe in the switching direction 0 = Measurement without spindle reversal, without probe alignment 1 = Measurement with spindle reversal 2 = Align probe in switching direction 302 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

301 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning 2 Selection S_KNUM Correction of the work offset (WO) or basic WO or basic reference 2) Cycle parameters Values: UNITS: TENS: 0 = No correction 1 to max. 99 numbers of the work offset or 1 to max. 16 numbers of the basic offset HUNDREDS: Reserved THOUSANDS: Correction of WO or basic or basic reference 0 = Correction of the adjustable WO 1 = Correction of the channel-specific basic WO 2 = Correction of the basic reference 3 = Correction of the global basic WO 9 = Correction of the active WO or for G500 in last active channel-specific basic WO 0 = Fine correction 6) 1 = Coarse correction 3 Selection S_KNUM1 Correction in tool offset 2) 4 Icon+ number S_PRNUM TEN THOUSANDS: Coarse or fine correction in the WO, basic WO or basic reference Values: UNITS: TENS: HUNDREDS: 0 = No correction 1 to max. 999 D numbers (cutting edge numbers) for tool offset; for additive and setup offset, see also S_DLNUM THOUSANDS: 0 or unique D numbers TEN THOUSANDS: 0 or unique D numbers 1 to max if unique D numbers in MDs have been set up HUNDRED THOUSANDS: Tool offset 2) 0 = No specification (offset in tool radius) 1 = Offset of length L1 2 = Offset of length L2 3 = Offset of length L3 4 = Radius offset ONE MILLION: Tool offset 2) 0 = No specification (offset of the tool radius wear) 1 = Tool offset, additive offset (AO) 5) Tool offset value is added to the existing AO 2 = Tool offset, setup offset (SO) 5) SO (new) = SO (old) + AO (old) offset value, AO (new) = 0 3 = Tool offset, setup offset (SO) 5) Tool offset value is added to the existing SO 4 = Tool offset, geometry TEN MILLION: Tool offset 2) 0 = No specification (offset in tool geometry normal, not inverted) 1 = Offset inverted Number of the field of the probe parameter (not probe number) (value range 1 to 12) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 303

302 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Cycle parameters Meaning 5 X0 S_SETV Setpoint 6 DFA S_FA Measurement path 7 TSA S_TSA Safe area 8 X0 S_CPA Center point of the 1st axis of the plane (for G17 X) 9 Y0 S_CPO Center point of the 2nd axis of the plane (for G17 Y) 10 alpha 0 S_STA1 Starting angle 7) 11 Alpha 1 S_INCA Incremental angle 8) S_NMSP Number of measurements at the same location 1) (value range 1 to 9) 13 T S_TNAME Tool name 2) 14 DL S_DLNUM Setup additive offset DL number 1), 2) 15 TZL S_TZL Work offset 16 DIF S_TDIF Dimensional difference check 17 TUL S_TUL Upper tolerance limit (incremental to the setpoint) 2) 18 TLL S_TLL Lower tolerance limit (incremental to the setpoint) 2) 19 TMV S_TMV Offset range for averaging 1) 20 FW S_K Weighting factor for averaging 1) 21 S_EVNUM Date set, empirical value memory 22 S_MCBIT Reserved 23 _DMODE Display mode 24 _AMODE Alternative mode 12 Measurements Values: Values: 1), 2) 1), 4) 1), 6) UNITS: Machining plane G17/G18/G19 0 = Compatibility, the plane active before the cycle call remains active 1 = G17 (only active in the cycle) 2 = G18 (only active in the cycle) 3 = G19 (only active in the cycle) UNITS: Dimensional tolerance yes/no 0 = No 1 = Yes 0) All default values = 0 or marked as the range of values a to b 1) Display depends on the general SD $SNS_MEA_FUNCTION_MASK_PIECE 2) Only for offset in tool, otherwise parameter = "" 3) Only for offset in tool and dimensional tolerance "Yes", otherwise parameter = 0 4) Only if the "Setup additive offset" function has been set-up in the general MD $MN_MM_NUM_SUMCORR. 5) If WO "fine" has not been set up in MDs, correction is made according to WO "coarse" 6) Empirical averaging only possible for tool offset Value range for empirical mean value memory: 1 to 20 numbers (n) of the empirical value memory, see channel-specific SD $SCS_MEA_EMPIRIC_VALUE[n-1] to numbers (n) of the mean value memory, see channel-specific SD $SCS_MEA_AVERAGE_VALUE[n-1] 7) Value range of starting angle -360 to +360 degrees 8) Value range of incremental angle >0 to 90 degrees for four measuring points or >0 to 120 degrees for three measuring points. 304 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

303 Parameter lists 4.1 Overview of measuring cycle parameters CYCLE997 measuring cycle parameters PROC CYCLE997 (INT S_MVAR,INT S_KNUM,INT S_PRNUM,REAL S_SETV,REAL S_FA,REAL S_TSA,REAL S_STA1,REAL S_INCA,REAL S_SETV0,REAL S_SETV1,REAL S_SETV2,REAL S_SETV3,REAL S_SETV4,REAL S_SETV5,REAL S_SETV6,REAL S_SETV7,REAL S_SETV8,REAL S_TNVL,INT S_NMSP,INT S_MCBIT,INT _DMODE,INT _AMODE) Table 4-10 CYCLE997 call parameters No. Screen form parameters Meaning 1), 2) 1 S_MVAR Measuring variant (default =9) Cycle parameters Values: UNITS: Contour element 9 = Measure sphere TENS: Repeat measurement 0 = Without measurement repetition 1 = With measurement repetition HUNDREDS: Correction target 0 = Only measurement (no correction of WO) 1 = Measurement, determination and correction of the WO (see S_KNUM) THOUSANDS: Measuring strategy 0 = Paraxial measurement, without starting angle, probe alignment corresponding to SD55740, bit 1 1 = Circling measurement, with starting angle, probe alignment corresponding to SD55740, Bit 1 2 = Circling measurement, with starting angle, align probe in the switching direction 3 = Paraxial measurement, with starting angle, probe alignment corresponding to SD55740, bit 1 4 = Paraxial measurement, with starting angle, align probe in the switching direction TEN THOUSANDS: Number of spheres to be measured 0 = Measure one sphere 1 = Measure three spheres HUNDRED THOUSANDS: Number of measuring points, only for measurement at an angle (note measuring strategy: THOUSANDS position > 0) 0 = Three measuring points for measurement at an angle (traversing around the sphere) 1 = Four measuring points for measurement at an angle (traversing around the sphere) ONE MILLION: Determination of the diameter setpoint of the sphere 0 = No determination of the diameter setpoint of the sphere 1 = Determination of the diameter setpoint of the sphere Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 305

304 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning 2 Selection S_KNUM Correction in work offset (WO) or basic or basic reference 3) 3 Icon+ number S_PRNUM Cycle parameters Values: UNITS: TENS: 0 = No correction 1 to max. 99 numbers of the work offset or 1 to max. 16 numbers of the basic offset HUNDREDS: Reserved THOUSANDS: Correction in WO or basic WO or basic reference 0 = Correction in the adjustable WO 1 = Correction in the channel-specific basic WO 2 = Correction in the basic reference 3 = Correction in the global basic WO 7) 9 = Correction in the active WO or for G500 in the last active channel-specific basic WO TEN THOUSANDS: Coarse or fine correction in the WO or basic WO or basic reference 0 = Fine correction 6) 1 = Coarse correction 4 S_SETV Diameter of the sphere(s) 4) 5 DFA S_FA Measurement path 6 TSA S_TSA Safe area Number of the field of the probe parameter (not probe number) (value range 1 to 12) 7 Alpha 0 S_STA1 Starting angle for measurement at an angle 8 Alpha 1 S_INCA Incremental angle for measurement at an angle 9 X1 S_SETV0 Position setpoint of the 1st sphere of the 1st axis of the plane (for G17 X) for 3 sphere measurement 10 Y1 S_SETV1 Position setpoint of the 1st sphere of the 2nd axis of the plane (for G17 Y) for 3 sphere measurement 11 Z1 S_SETV2 Position setpoint of the 1st sphere of the 3rd axis of the plane (for G17 Z) for 3 sphere measurement 12 X2 S_SETV3 Position setpoint of the 2nd sphere of the 1st axis of the plane for 3 sphere measurement 13 Y2 S_SETV4 Position setpoint of the 2nd sphere of the 2nd axis of the plane for 3 sphere measurement 14 Z2 S_SETV5 Position setpoint of the 2nd sphere of the 3rd axis of the plane for 3 sphere measurement 15 X3 S_SETV6 Position setpoint of the 3rd sphere of the 1st axis of the plane for 3 sphere measurement 16 Y3 S_SETV7 Position setpoint of the 3rd sphere of the 2nd axis of the plane for 3 sphere measurement 17 Z3 S_SETV8 Position setpoint of the 3rd sphere of the 3rd axis of the plane for 3 sphere measurement 18 TVL S_TNVL Limit value for distortion of the triangle (sum of the deviations) for 3 sphere measurement 5) 19 Measurements S_NMSP Number of measurements at the same location 2) (value range 1 to 9) 20 S_MCBIT Reserved 306 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

305 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning 21 _DMODE Display mode Cycle parameters Values: 22 _AMODE Alternative mode UNITS: Machining plane G17/G18/G19 1) All default values = 0 or marked as the range of values a to b 0 = compatibility, the plane active before the cycle call remains active 1 = G17 (only active in the cycle) 2 = G18 (only active in the cycle) 3 = G19 (only active in the cycle) 2) Display depends on the general SD $SNS_MEA_FUNCTION_MASK_PIECE 3) Intermediate positioning, circling around the ball at the equator 4) 3 sphere measurement: The same diameter setpoint applies for all three spheres (_SETV) 5) Default value for S_TNVL=1.2 Correction in WO: Correction is only performed in the WO when the determined distortion is below the S_TNVL limit value. 6) If WO "fine" has not been set up in MDs, correction is according to WO "coarse" 7) For measuring variant "Measure three spheres", correction in a global basic frame is not possible (S_KNUM = 3001 to 3016), as the frame does not have a rotation component CYCLE995 measuring cycle parameters PROC CYCLE995 (INT S_MVAR,INT S_KNUM,INT S_PRNUM,REAL S_SETV,REAL S_FA,REAL S_TSA,REAL S_STA1,REAL S_INCA,REAL S_DZ,REAL S_SETV0,REAL S_SETV1,REAL S_SETV2,REAL S_TUL,REAL S_TZL,INT S_NMSP,INT S_MCBIT,INT _DMODE,INT _AMODE) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 307

306 Parameter lists 4.1 Overview of measuring cycle parameters Table 4-11 CYCLE995 call parameters 1) No. Screen form parameters Meaning 1 S_MVAR Measuring variant (default=5) 2 Selection S_KNUM Correction target 3 Icon+ number S_PRNUM 0 = 0 UNITS: Contour element 5 = Spindle geometry (parallel to the tool axis) TENS: Repeat measurement 1 = with repeat measurement HUNDREDS: No offset target 0 = measurement only THOUSANDS: Measuring strategy 2 = measurement at an angle, align measuring probe in direction of switching TEN THOUSANDS: Number of spheres to be measured 0 = measure a sphere HUNDRED THOUSANDS: Number of measurement points 1 = 4 measurement points when measuring at an angle (circle the sphere) ONE MILLION: Determination of the diameter setpoint of the sphere 0 = No determination of the diameter setpoint of the sphere 1 = Determination of the diameter setpoint of the sphere Number of the field of the probe parameter (not probe number) (value range 1 to 12) 4 DM S_SETV Diameter of the calibration ball 4) 5 DFA S_FA Measurement path 6 TSA S_TSA Safe area 5) 7 alpha 0 S_STA1 Starting angle for measurement at an angle 3) 8 S_INCA Incremental angle for measurement at an angle 2) 9 DZ S_DZ Distance 1st measurement P1 to the 2nd measurement P2 after the shaft of the probe 10 S_SETV0 Setpoint position of the ball of the 1st axis of the plane (for G17 X) 2) 11 S_SETV1 Setpoint position of the ball of the 2nd axis of the plane (for G17 Y) 2) 12 S_SETV2 Setpoint position of the ball of the 3rd axis of the plane (for G17 Z) 2) 13 TUL S_TUL Upper tolerance value of the angle values 1), 4) 14 TZL S_TZL Zero offset range 15 Number S_NMSP Number of measurements at the same location 2) (value range 1 to 9) 16 S_MCBIT Reserved 2) 17 _DMODE Display mode Cycle parameters Values: Values: UNITS: Machining plane G17/G18/G19 0 = compatibility, the plane active before the cycle call remains active 1 = G17 (only active in the cycle) 2 = G18 (only active in the cycle) 3 = G19 (only active in the cycle) 308 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

307 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning 18 _AMODE Alternative mode Cycle parameters Values: UNITS: Dimensional tolerance yes/no 0 = No 1 = Yes All default values = 0 or marked as the range of values a to b 1) Display depends on the general SD54760 $SNS_MEA_FUNCTION_MASK_PIECE 2) Parameters are currently not used and also not displayed in the input screen. The parameter incremental angle S_INCAis permanently set to 90 degrees. 3) Value range of starting angle -360 to +360 degrees 4) for dimensional tolerance yes: If the measured angle is less than the value of the work offset range TZL, then the result parameters for the angle (_OVR[2], _OVR[3]) and deviations (_OVR[7], _OVR[8]) are set to zero. DisplayTZL is realized using the general SD54760 $SNS_MEA_FUNCTION_MASK_PIECE bit25=1. (enable selected zero offset when measuring angularity, spindle) 5) Parameter TSA refers to the 1st measurement of the calibration ball CYCLE996 measuring cycle parameters PROC CYCLE996(INT S_MVAR,INT S_TC,INT S_PRNUM,REAL S_SETV,REAL S_STA1,REAL S_SETV0,REAL S_SETV1,REAL S_SETV2,REAL S_SETV3,REAL S_SETV4,REAL S_SETV5,REAL S_TNVL,REAL S_FA,REAL S_TSA,INT S_NMSP,INT S_MCBIT,INT _DMODE,INT _AMODE) Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 309

308 Parameter lists 4.1 Overview of measuring cycle parameters Table 4-12 CYCLE996 call parameters 1) No. Screen form parameters Meaning 1 S_MVAR Measurement version (default=1) Cycle parameters Values: UNITS: Measuring sequence 0 = Calculate kinematics (selection with: Result display, protocol, change of the swivel data sets, where relevant with operator acknowledgment), see _AMODE 1 = 1st measurement 2 = 2nd measurement 3 = 3rd measurement TENS: Reserved 0 = 0 HUNDREDS: Measurement version for 1st to 3rd measurement 0 = Measurement of the calibration ball paraxial 1 = Measurement of the calibration sphere at an angle and no spindle correction 3) 2 = Measurement of the calibration sphere and correction of the spindle in the switching direction of the probe 3) 3 = Paraxial measurement, with starting angle 8) 4 = Paraxial measurement, with starting angle, tracking spindle in the switching direction of the probe 8) THOUSANDS: Calculate correction target for kinematics 4) 0 = measuring only. Swivel data sets are calculated, but remain unchanged 1 = calculate swivel data set. Swivel data sets are, if necessary, changed after acknowledgment by the operator 4) TEN THOUSANDS: Measuring axis (rotary axis 1 or 2) or vector chain open or closed for calculate kinematics 0 = Vector chain closed (only for calculate kinematics) 1 = Rotary axis 1 (only for 1st to 3rd measurement) 2 = rotary axis 2 (only for the 1st to 3rd measurement) 5) 3 = vector chain open (only for calculate kinematics) HUNDRED THOUSANDS: Normalizing of rotary axis 1 for calculate kinematics 0 = no scaling rotary axis 1 1 = scaling in the direction of the 1st axis of the plane (for G17 X) 2 = scaling in the direction of the 2nd axis of the plane (for G17 Y) 3 = scaling in the direction of the 3rd axis of the plane (for G17 Z) ONE MILLION: Normalizing of rotary axis 2 for calculate kinematics 5) 0 = no scaling rotary axis 2 1 = scaling in the direction of the 1st axis of the plane (for G17 X) 2 = scaling in the direction of the 2nd axis of the plane (for G17 Y) 3 = scaling in the direction of the 3rd axis of the plane (for G17 Z) TEN MILLION: Log file 2 S_TC Number of the swivel data record (tool carrier) 3 Icon+ number S_PRNUM 0 = no protocol file 1 = protocol file with the calculated vectors (tool carrier) and the 1st dynamic 5- axis transformation (TRAORI(1)), if set-up in MDs. Number of the field of the probe parameters (not probe number) (default=1) 310 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

309 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Cycle parameters Meaning 4 S_SETV Diameter of the calibration ball 5 alpha 0 S_STA1 Starting angle for measurement at an angle 6 alpha 0 S_SETV0 Position value of rotary axis 1 (if rotary axis is manual or semi-automatic) 7 alpha 1 S_SETV1 Position value of rotary axis 2 (if rotary axis is manual or semi-automatic) 6) 8 XN S_SETV2 Position value for normalizing rotary axis 1 9 XN S_SETV3 Position value for normalizing of rotary axis 2 6) 10 Delta S_SETV4 Tolerance value of the offset vectors I1 to I4 11 Delta S_SETV5 Tolerance value of rotary axis vectors V1 and V2 12 TVL S_TNVL Limit value of angular segment of the rotary axis (value range 1 to 60 degrees) (default=20) 7) 13 DFA S_FA Measurement path 14 TSA S_TSA Safe area S_NMSP 16 S_MCBIT Reserved 17 _DMODE Display mode Number of measurements at the same location 2) (default=1) 18 _AMODE Alternative mode 15 Measurements Values: Values: UNITS: Machining plane G17/G18/G19 0 = compatibility, the plane active before the cycle call remains active 1 = G17 (only active in the cycle) 2 = G18 (only active in the cycle) 3 = G19 (only active in the cycle) UNITS: Tolerance check yes/no 0 = No 1 = Yes: Evaluation of the tolerance values of the vectors S_SETV4, S_SETV5 TENS: Acknowledgment by the operator when entering the calculated vectors in the swivel data set 4) 0 = yes: Operator must acknowledge the change 1 = no: calculated vectors are entered immediately (only effective if HUNDREDS and THOUSANDS position = 0) HUNDREDS: Measurement result display 5) 0 = no 1 = yes 1) All default values = 0 or marked as default=x THOUSANDS: Measurement result display can be edited 0 = no 1 = yes, and can be edited (only effective, if the HUNDREDS position = 1) 2) Display depends on the general SD54760 $SNS_MEA_FUNCTION_MASK_PIECE 3) Using this version, for example, for 90 degree positions, the kinematics can be measured at the calibration ball, without colliding with the retaining shaft of the calibration ball. A starting angle S_STA1 (0 to 360 degrees) can be entered. The incremental angle when circling the sphere is equal to 90 degrees. As feedrate along the circular path, the channel-specific SD55634 $SCS_MEA_FEED_PLANE_VALUE is used 4) There is an operator prompt with M0 before entering. The vectors are only entered with NC start. If the measuring program is aborted with RESET no calculated vectors are entered. Vectors are only entered when the tolerance of the offset vectors has not been exceeded during the calculation. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 311

310 Parameter lists 4.1 Overview of measuring cycle parameters 5) Measurement result display only for the calculated kinematics measuring version. If the measurement result should also be displayed after the 1st to the 3rd measurement, then this is realized by setting the channel-specific SD $SCS_MEA_RESULT_DISPLAY. 6) Rotary axis 2 only for kinematics with two rotary axes 7) Limit value angular segment of the rotary axis. Value range of S_TNVL between 20 and 60 degrees. For values of S_TNVL < 20 degrees, inaccuracies can be expected as a result of the measuring inaccuracies in the micrometer range of the probe. If the limit value is violated, then error message is output with a display of the minimum limit value. 8) Spindle is tracked in the probe switching direction if SD54760 bit 17 = CYCLE982 measuring cycle parameters PROC CYCLE982(INT S_MVAR,INT S_KNUM,INT S_PRNUM,INT S_MA,INT S_MD,REAL S_ID,REAL S_FA,REAL S_TSA,REAL S_VMS,REAL S_STA1,REAL S_CORA,REAL S_TZL,REAL S_TDIF,INT S_NMSP,INT S_EVNUM,INT S_MCBIT,INT _DMODE,INT _AMODE) 312 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

311 Parameter lists 4.1 Overview of measuring cycle parameters Table 4-13 CYCLE982 call parameters 1) No. Screen form parameters Meaning 1 S_MVAR Measuring version 2 Selection S_KNUM Offset variant 2) 3 Icon+ number S_PRNUM 4 X0 S_MA Measuring axis UNITS: Calibration/measurement 0 = Calibrate tool probe 1 = Single tool measurement 3) 2 = Multiple tool measurement, determine lengths and tool radius (for milling tools) TENS: Calibration or measurement in the MCS or WCS 0 = Machine-related 4) 1 = Workpiece-related HUNDREDS: Measurement with or without reversal for milling tools 0 = Measurement without reversal 1 = Measurement with reversal THOUSANDS: Correction target for milling tools 0 = determine length or length and radius (see S_MVAR 1st position) 1 = determine radius, if S_MVAR 1st position = 1 2 = determine length and radius (face side), if S_MVAR 1st position = 1 or 2 3 = side milling tool, upper cutting edge (rear side) and determine length and radius 5) TEN THOUSANDS: Position of the milling tool or the drill 0 = Axial position of the milling tool or the drill, radius in 2nd axis of the plane (for G18 X) 7) 1 = Radial position of the milling tool or the drill, radius in 1st axis of the plane (for G18 Z) 7) HUNDRED THOUSANDS: Incremental calibration or measurement 0 = No specification 1 = Incremental calibration or measurement ONE MILLION: Position spindle at starting angle S_STA1 (only for measurement of milling tools) 0 = spindle is not positioned 1 = spindle is positioned at the starting angle S_STA1 UNITS: Tool offset 0 = No specification (tool offset in geometry) 1 = Tool offset in wear Number of the field of the probe parameters (not probe number) (default=1) 5 +- S_MD Measuring direction Cycle parameters Values: Values: Values: Values: 1 = 1. Axis of the plane (for G18 Z) 2 = 2nd axis of the plane (for G18 X) 0 = No selection (measuring direction is determined from actual value) 1 = Positive 2 = Negative Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 313

312 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Cycle parameters Meaning 6 Z2 S_ID Offset 7 DFA S_FA Measurement path 8 TSA S_TSA Safe area 9 VMS S_VMS Variable measuring velocity for calibration 2) 10 Alpha1 S_STA1 Starting angle when measuring milling tools 11 Alpha2 S_CORA Offset angle when measuring milling tools with reversal 8) 12 TZL S_TZL Work offset when measuring milling tools When calibrating S_TZL = 0 13 DIF S_TDIF Dimension difference check S_NMSP Number of measurements at the same location 2) (default=1) 15 EVN S_EVNUM Number of the empirical mean value memory 16 S_MCBIT Reserved 17 _DMODE Display mode 2), 9) UNITS: Machining plane G17/G18/G19 0 = Compatibility, the plane active before the cycle call remains active 1 = G17 (only active in the cycle) 2 = G18 (only active in the cycle) 3 = G19 (only active in the cycle) TENS: Cutting edge position for turning and milling tools (only for display in the input screens 1 to 9) HUNDREDS: Tool type 0 = Turning tool 1 = Milling tool 2 = Drill 18 _AMODE Alternative mode 14 Measurements Values: Values: 1) All default values = 0 or marked as default=x THOUSANDS: The approach strategy with reference to the tool probe 0 = PLUS [X/Z]; X if tool position axial, Z if tool position radial 1 = MINUS [X/Z]; X if tool position axial, Z if tool position radial UNITS: Reserved TENS: Reserved HUNDREDS: Reserved THOUSANDS: approach starting position after measurement for calibration and single measurement (see S_MVAR - UNITS) 0 = tool is located, offset by DFA with respect to the probe edge 1 = approach starting position 2) Display depends on the general SD _MEA_FUNCTION_MASK_TOOL 3) Measure turning or milling tool or drill. Measuring axis in parameter S_MA Specification for turning tools via cutting edge position 1...8, for milling tools via HUNDREDS to THOUSANDS position in parameter S_MVAR. 4) Measurement and calibration are performed in the basic coordinate system (MCS for kinematic transformation switched off). 5) Not for incremental measuring 314 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

313 Parameter lists 4.1 Overview of measuring cycle parameters 6) Only for multiple measurements S_MVAR=x2x02 or x3x02 (example, disk-type or groove milling tools) 7) If the channel-specific SD $SC_TOOL_LENGTH_TYPE = 2, then the tool length components are assigned just the same as for turning tools 8) Only for measurement with reversal S_MVAR=xx1x1 9) Empirical value generation Value range of the empirical value memory: 1 to 20 numbers(n) of the empirical value memory, see channel-specific SD $SCS_MEA_EMPIRIC_VALUE[n-1] CYCLE971 measuring cycle parameters PROC CYCLE971(INT S_MVAR,INT S_KNUM,INT S_PRNUM,INT S_MA,INT S_MD,REAL S_ID,REAL S_FA,REAL S_TSA,REAL S_VMS,REAL S_TZL,REAL S_TDIF,INT S_NMSP,REAL S_F1,REAL S_S1,REAL S_F2,REAL S_S2,REAL S_F3,REAL S_S3,INT S_EVNUM,INT S_MCBIT,INT _DMODE,INT _AMODE) Table 4-14 CYCLE971 call parameters 1) No. Screen form parameters Meaning 1 S_MVAR Measuring version Cycle parameters Values: UNITS: 0 = Calibrate tool probe 1 = Measure tool with stationary spindle (length or radius) 2 = Measure tool with rotating spindle (length or radius), see parameters S_F1 to S_S4 TENS: Measurement in the machine coordinate system or workpiece coordinate system 0 = Measurement in MCS (machine-related), measure tool or calibrate tool probe 1 = Measurement in WCS (workpiece-related), measure tool or calibrate tool probe HUNDREDS: Tooth breakage monitoring for milling cutters 0 = no 1 = yes THOUSANDS: 0 = 0 TEN THOUSANDS: Incremental calibration or measurement 0 = No specification 1 = Incremental calibration or measurement HUNDRED THOUSANDS: Calibrate tool probe automatically 0 = Do not calibrate tool probe automatically 1 = Calibrate tool probe automatically ONE MILLION: Calibrating in the plane with spindle reversal 0 = Calibrating in the plane without spindle reversal 1 = Calibrating in the plane with spindle reversal Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 315

314 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning 2 Selection S_KNUM Offset variant 2) 3 Icon+ number S_PRNUM UNITS: Tool offset 4 X0 S_MA Measuring axis, offset axis 4) 0 = No specification (tool offset in geometry) 1 = Tool offset in wear Number of the field of the probe parameters (not probe number) UNITS: Number of the measuring axis 1 = 1st axis of the plane (for G17 X) 2 = 2nd axis of the plane (for G17 Y) 3 = 3rd axis of the plane (for G17 Z) TENS: 0 = S_MD Measuring direction 6 V S_ID Offset Cycle parameters Values: Values: Values: Values: 7 DFA S_FA Measurement path 8 TSA S_TSA Safe area HUNDREDS: Number of the offset axis 0 = No offset axis 1 = 1st axis of the plane (for G17 X) 2 = 2nd axis of the plane (for G17 Y) 0 = No selection (measuring direction is determined from actual value) 1 = Positive 2 = Negative 0 = For tools without offset >0 = 9 VMS S_VMS Variable measuring velocity for calibration 2) 10 TZL S_TZL Work offset (only for tool measurement) Calibration: The offset is applied to the 3rd axis of the plane (for G17 Z) if the diameter of the calibration tool is greater than the upper diameter of the probe. The tool is offset by the tool radius from the center of the probe, minus the value of S_ID. The offset axis is also specified in S_MA. Measure: With multiple cutting edges, the offset of tool length and the highest point of the cutting edge must be specified for radius measurement or the offset of tool radius to the highest point of the cutting edge must be specified when measuring the length. 11 DIF S_TDIF Dimensional difference check for tool measurement (S_MVAR=xx1or S_MVAR=xx2) 12 Measurements S_NMSP Number of measurements at the same location 2) 13 F1 S_F1 1st feedrate for contact with rotating spindle 2) 14 S1 S_S1 1st speed for contact with rotating spindle 2) 15 F2 S_F2 2nd feedrate for contact with rotating spindle 2) 16 S2 S_S2 2nd speed for contact with rotating spindle 2) 17 F3 S_F3 2nd feedrate for contact with rotating spindle 3) 316 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

315 Parameter lists 4.1 Overview of measuring cycle parameters No. Screen form parameters Meaning 18 S3 S_S3 2nd speed for contact with rotating spindle 3) 19 EVN S_EVNUM Number of the empirical value memory 2) 20 S_MCBIT Screen form of the _CBITs or _CHBITs 21 _DMODE Display mode 22 _AMODE Alternative mode Cycle parameters Values: Values: UNITS: Machining plane G17/G18/G19 0 = Compatibility, the plane active before the cycle call remains active 1 = G17 (only active in the cycle) 2 = G18 (only active in the cycle) 3 = G19 (only active in the cycle) UNITS: Measuring the tool offset for radius 1 = no 2 = yes 1) All default values = 0 or marked as default=x TENS: Direction of the tool offset when measuring the radius in the 3rd axis of the plane (for G17 Z) 1 = Positive 2 = Negative HUNDREDS: Tool offset when measuring the length or when calibrating the probe in the 3rd axis 0 = Compatibility, auto 1 = No 2 = Yes THOUSANDS: Direction of the tool offset when measuring the length in the offset axis (see S_MA HUNDREDS) 1 = Positive 2 = Negative 2) Display depends on the general SD MEA_FUNCTION_MASK_TOOL 3) Only for offset in tool and dimensional tolerance "Yes", otherwise parameter = 0 4) For automatic measurement (S_MVAR=1x00xx), no display of measuring axis, offset axis S_MA= CYCLE150 measuring cycle parameters PROC CYCLE150(INT S_PICT,INT S_PROT,STRING[160] S_PATH) SAVE ACTBLOCNO DISPLOF Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 317

316 Parameter lists 4.1 Overview of measuring cycle parameters Table 4-15 CYCLE150 call parameters No. Screen parameters 1 Measuring result screen Cycle parameters Meaning S_PICT Select result display (default = 0) Values: UNITS: 0 = Measuring result screen OFF 1 = Measuring result screen ON 2 S_PROT Select logging (default = 0) Tens: Select display mode (values as for SD 55613) 1 = Display measuring result screen - automatically deselect after 8 s 3 = Display measuring result screen - acknowledge using NC Start 4 = Display measuring result screen - only for alarms ( ) Log Values: UNITS: Select protocol off / on / last measurement 0 = Log OFF 1 = Log ON 2 = Log last measurement Log type TENS: Select log type 0 = Standard log 1 = User log (can be freely defined) Log format HUNDREDS: Select log format 0 = Text format 1 = Table format (for import to Excel) Log data THOUSANDS: Rewrite or attach selection Log archive 0 = New 1 = Attach TEN THOUSANDS: Select log archive 0 = As part program 1 = Directory 3 S_PATH Path for the log file corresponding to the log archive selection (complete path name or only file name, e.g.: "//NC:/WKS.DIR/NAME.WPD or "MESSPROTOKOLL.TXT" 318 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

317 Parameter lists 4.2 Additional parameters 4.2 Additional parameters The following supplementary parameters can be hidden or unhidden using setting data in the input screen forms. For more information about setting data SD54760 to SD54764, see the List Manual SINUMERIK 840D sl, detailed description of the machine data. Machine manufacturer Please observe the machine manufacturer s instructions. The supplementary parameter are not available for all measuring cycles. See also the interface description. Table 4-16 Supplementary parameters for workpiece measurement Screen form parameters Transfer parameters Description Calibration data set S_PRNUM Number of the data set with the calibrated values of the probe - F S_VMS Measuring feedrate when calibrating the probe mm/min Selection S_MVAR Calibrate probe: selection at the known or unknown center point of the calibration ring Selection S_MVAR Calibrate probe: selection, calibration with or without position deviation (probe skew) Number S_NMSP Number of measurements at the same location - TZL S_TZL Work offset for correction in a tool mm DIF S_TDIF Dimension difference monitoring for correction in a tool - Data set, mean value generation Data set, empirical values S_EVNUM Generating mean values for correction in a tool - S_EVNUM Generating empirical values for correction in a tool - FW S_K Weighting factor for averaging - TMV S_TMV Offset range for averaging Selection S_MVAR Measuring when turning, diameter inside outside: With reversal Travel under center of rotation Unit Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 319

318 Parameter lists 4.2 Additional parameters Additional correction options when measuring workpiece: 1. Work offsets Offset in the basic reference Offset in the channel-specific basic WO Offset in the global basic WO Offset, coarse or fine 2. Tool offsets Tool offset in geometry or wear Tool offset, inverted or not inverted Tool offset in radius or length L1 or L2 or L3 Table 4-17 Supplementary parameter when measuring tool Screen form parameters Transfer parameters Description Calibration data set S_PRNUM Number of the data set with the calibrated values of the probe - F S_VMS Measuring feedrate when calibrating the probe mm/min Selection, measuring steps S_MVAR Input of max. 3 feedrates and 3 spindle speeds when measuring with rotating spindle Selection S_MVAR Tool offset in geometry or wear - Selection S_MVAR Measurement in the machine coordinate system or workpiece coordinate system Number S_NMSP Number of measurements at the same location - Data set, empirical values S_EVNUM Generating empirical values for correction in a tool - Unit Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

319 Parameter lists 4.3 Additional result parameters 4.3 Additional result parameters The following table below contains the additional result parameters for the measuring variants of the tool offset. Parameters Description Unit _OVR [8] 1) _OVR [9] 1), 3) Upper _OVR [12] 1) 1), 3) _OVR [13] Lower Upper tolerance limit for: Diameter of hole / circular spigot / circle segment Measuring axis Width of groove/rib Rectangle length in the 1st axis of the plane tolerance limit for rectangle length in the 2nd axis of the plane Lower tolerance limit for: Diameter of hole / circular spigot / circle segment Measuring axis Width of groove/rib Rectangle length in the 1st axis of the plane tolerance limit for rectangle length in the 2nd axis of the plane _OVR [20] 1) Offset value mm _OVR [27] 1) Work offset range mm _OVR [28] 1) Safe area mm _OVR [29] 1) Dimensional difference mm _OVR [30] 1) Empirical value mm _OVR [31] 1) Mean value mm _OVI [4] 1) Weighting factor - _OVI [5] Probe number - _OVI [6] 1) Mean value memory number - _OVI [7] 1) Empirical value memory number - _OVI [8] 1) Tool number - _OVI [9] 1) Alarm number - _OVI [11] 2) Status offset request - _OVI [13] 1) DL number - 1) Only for workpiece measurement with tool offset 2) only for correction in the WO 3) Only applies for the measuring versions "Rectangular pocket" and "Rectangular spigot" mm mm mm mm Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 321

320 Parameter lists 4.4 Parameter 4.4 Parameter Table 4-18 List of input/output variables for cycles Screen form parameters Cycle parameters Meaning in English Meaning in German S_CALNUM Calibration groove number Number of the gauging block S_MCBIT Central Bits Screen form of the _CBITs or _CHBITs α2 S_CORA Correction angle position Offset angle X0 S_CPA Center point abscissa Center point of the 1st axis of the plane Y0 S_CPO Center point ordinate Center point of the 2nd axis of the plane DL S_DLNUM DL number for setup or additive offset EVN S_EVNUM Number, mean empirical value memory DFA S_FA Factor for multipl. of measurem. path Measurement path S_ID Infeed in applicate Incremental infeed absolute value / offset α1 S_INCA Indexing angle Incremental angle / angle setpoint FW S_K Weighting factor for averaging Weighting factor for averaging Selection S_KNUM Correction WO, basic WO or basic reference Selection S_KNUM1 Correction in tool offset X / Y / Z S_MA Number of measuring axis Measuring axis (number of the axis) + / - S_MD Measuring direction Measuring direction S_MFS Feedrate and speed for measurement with rotating spindle S_MVAR Measuring variant Measuring version Number S_NMSP Number of measurements at same spot _OVI [20] _OVR [32] Number of measurements at the same location Field: Output values INT Field: Output values REAL Icon + number S_PRNUM Probe type and probe number Number of the field of the probe parameters X0 / Y0 / Z0 S_SETV Setpoint value Setpoint α1 S_STA1 Starting angle Starting angle X S_SZA Safety zone on workpiece abscissa Protection zone in the 1st axis of the plane Y S_SZO Safety zone on workpiece ordinate Protection zone in the 2nd axis of the plane DIF S_TDIF Tolerance dimensional difference check Dimension difference check TLL S_TLL Tolerance lower limit Tolerance lower limit TMV S_TMV Mean value generation with compensation T S_TNAME Tool name Tool name when using tool manager S_TNVL Limit value for distortion of the triangle TSA S_TSA Tolerance safe area Safe area TUL S_TUL Tolerance upper limit Tolerance upper limit TZL S_TZL Tolerance zero offset range Work offset VMS S_VMS Variable measuring speed Variable measuring speed 322 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

321 Parameter lists 4.4 Parameter Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 323

322 Parameter lists 4.4 Parameter 324 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

323 Changes from cycle version SW4.4 and higher A A.1 Assignment of the measuring cycle parameters to MEA_FUNCTION_MASK parameters Bit 1) Function All setting data that were saved up to measuring cycle version 2.6 in GUD variables, from software release SW 4.4 are located in the configurable machine and setting data (e.g. data fields of the calibration values). The GUD modules GUD5, GUD6 and GUD7_MC are no longer required for measuring cycle data. The following tables include the assignment of function-determining measuring cycle parameters to the MEA_FUNCTION_MASK parameters. MD identifier SW 2.6 General cycle machine data: MD51740 $MNS_MEA_FUNCTION_MASK (32 bits) Workpiece measurement GUD name up to SW Calibration monitoring (default = 1) $MNS_MEA_CAL_MONITORING _CBIT[16] 1 Length reference of the probe in the infeed axis (default = 1) 0 = Reference point is the center of the probe sphere 1 = Reference point is the circumference of the probe sphere 2 Taking into account tool carriers that can be orientated for offset in a tool (default = 0) 3 Offset angle for mono-workpiece probe (default = 1) Tool measurement 16 Taking into account tool carriers that can be orientated for offset in a tool (default = 0) $MNS_MEA_PROBE_LENGTH_RE LATE _CBIT[14] $MNS_MEA_TOOLCARR_ENABLE _CBIT[7] $MNS_MEA_MONO_COR_POS_AC TIVE MD $MNS_MEA_TOOLCARR_ENA BLE _CBIT[8] _CBIT[7] Channel-specific cycle machine data: MD52740 $MCS_MEA_FUNCTION_MASK (32 bits) Workpiece measurement 0 Measuring input, workpiece probe (default = 0) 0 = CNC measuring input 1 1 = CNC measuring input 2 1 Rotating measuring cycles use Y axis as measuring axis (default = 0) Tool measurement 16 Measuring input, tool probe (default = 1) 0 = CNC measuring input 1 1 = CNC measuring input $MNS_MEA_IN PUT_PIECE_PROBE[0] $MCS_MEA_TURN_CYC_SPE CIAL_MODE _CHBIT[0] _CHBIT[19] $MNS_MEA_INPUT_TOOL_PROBE[0] _CHBIT[1] General cycle setting data: SD $SNS_MEA_FUNCTION_MASK (32 bits) Workpiece measurement Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 325

324 Changes from cycle version SW4.4 and higher A.1 Assignment of the measuring cycle parameters to MEA_FUNCTION_MASK parameters Bit 1) Function 0 Repeat measurement in the event of violation of _TDIF and _TSA (default = 0) 1 Repeat measurement with alarm output and cycle stop at M0 (default = 0) 2 Violation of _TUL, _TLL, _TDI, cycle stop at M0 (default = 0) 3 Accept calibrated probe sphere radius in tool data (default = 1) Tool measurement 16 Repeat measurement in the event of violation of _TDIF and _TSA (default = 0) 17 Repeat measurement with alarm output and cycle stop at M0 (default = 0) 18 Violation of _TDIF, cycle stop at M0 (default = 0) 19 Milling cutter, spindle speed reduction at the last contact MD identifier SW 2.6 GUD name up to SW $SNS_MEA_REPEATE_ACTIVE _CBIT[0] $SNS_MEA_REPEATE_WITH_M0 _CBIT[1] $SNS_MEA_TOL_ALARM_SET_M0 _CBIT[2] $SNS_MEA_PROBE_BALL_RAD_IN_TOA _CBIT[15] $SNS_MEA_REPEATE_ACTIVE _CBIT[0] $SNS_MEA_REPEATE_WITH_M0 _CBIT[1] $SNS_MEA_TOL_ALARM_SET_M0 _CBIT[2] _CHBIT[22] Channel-specific setting data: SD $SCS_MEA_FUNCTION_MASK (32 bits) Workpiece measurement 0 Collision monitoring (default = 1) $SCS_MEA_COLLISION_MONITOR ING 1 Coupling of the spindle position, with a coordinate rotation around the infeed axis in AUTOMATIC (default = 0) 2 Direction of rotation of the spindle positioning, with active coupling of the spindle and coordinate rotation (default = 0) 0 = In the GUZ 1 = In the UZ 3 Measurement attempts when the probe does not switch (default = 0) 0 = 5 attempts 1 = 1 attempt 4 Approach velocity to the measuring position (default = 0) 0 = With measuring feedrate _VMS 1 = With $SCS_MEA_FEED_FAST_MEASURE 5 Retraction velocity from the measuring point (default = 0) 0 = With $SCS_MEA_FEED_PLANE_VALUE 1 = With $SCS_MEA_FEED_RAPID_IN_PERCENT _CHBIT[2] $SCS_MEA_COUPL_SPIND_COORD _CHBIT[13] $SCS_MEA_SPIND_MOVE_DIR _CHBIT[14] $SCS_MEA_NUM_OF_MEASURE _CHBIT[15] $SCS_MEA_FEED_TYP _CHBIT[17] $SCS_MEA_RETRACTION_FEED _CHBIT[16] 326 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

325 Changes from cycle version SW4.4 and higher A.1 Assignment of the measuring cycle parameters to MEA_FUNCTION_MASK parameters Bit 1) Function 6 Activate/deactivate workpiece probe before and after the NC command SPOS. See also CUST_MEA_CYC.SPF (default = 0)... 0 = No call CUST_MEA_CYC.SPF 1 = Call CUST_MEA_CYC.SPF 14 Coupling of the spindle position, with a coordinate rotation around the infeed axis when a measuring in AU TOMATIC (default = 1) 15 Calibration in the calibration ring when measuring in JOG (default = 0) 0 = Calibrate with automatic reference center point 1 = Calibrate with known reference center point Tool measurement MD identifier SW $SCS_J_MEA_SET_COUPL_SP_CO ORD GUD name up to SW 2.6 E_MESS_ SETT[0] $SCS_J_MEA_SET_CAL_MODE E_MESS_ SETT[1] 16 Collision monitoring (default = 1) $SCS_MEA_COLLISION_MONITOR ING 17 Measurement attempts when the probe does not switch (default = 0) 0 = 5 attempts 1 = 1 attempt 18 Approach velocity to the measuring position (default = 0) 0 = With measuring feedrate _VMS 1 = With $SCS_MEA_FEED_FAST_MEASURE 19 Retraction velocity from the measuring point (default = 0) 0 = With $SCS_MEA_FEED_PLANE_VALUE 1 = With $SCS_MEA_FEED_RAPID_IN_PERCENT 1) Bit x=0 means that the function is disabled Bit x=1 means that the function is enabled All non-documented bits are not assigned. _CHBIT[2] $SCS_MEA_NUM_OF_MEASURE _CHBIT[15] $SCS_MEA_FEED_TYP _CHBIT[17] $SCS_MEA_RETRACTION_FEED _CHBIT[16] Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 327

326 Changes from cycle version SW4.4 and higher A.2 Changes in the machine and setting data from SW 4.4 A.2 Changes in the machine and setting data from SW 4.4 MD replaced with SD MDs are no longer required The following cycle machine data (measuring in JOG) no longer apply from cycle release SW (compared to SW ) and are replaced by the following cycle setting data that mean the same. Replaced by SD $MNS_MEA_INPUT_TOOL_PROBE_SUB[0.. 5] $SNS_MEA_INPUT_TOOL_PROBE_SUB[0.. 5] $MNS_J_MEA_MEASURING_FEED $SCS_MEA_FEED_MEASURE $MNS_J_MEA_T_PROBE_TYPE[n] $SNS_MEA_TP_TYPE[n] $MNS_J_MEA_T_PROBE_ALLOW_AX_DIR[n] $SNS_MEA_TP_AX_DIR_AUTO_CAL[n] $MNS_J_MEA_T_PROBE_DIAM_LENGTH[n] $SNS_MEA_TP_EDGE_DISK_SIZE[n] $MNS_J_MEA_T_PROBE_T_EDGE_DIST[n] $SNS_MEA_TP_CAL_MEASURE_DEPTH[n] $MNS_J_MEA_T_PROBE_MEASURE_FEED $SCS_MEA_TP_FEED_MEASURE Change, number of the setting data For the following cycle setting data, from SW , the number of the setting data changes (with respect to cycle release SW ). Identifier and function have not changed. Number SD Release SW From SW Identifier $SNS_J_MEA_FUNCTION_MASK_PIECE $SNS_J_MEA_FUNCTION_MASK_TOOL $SCS_MEA_FEED_RAPID_IN_PERCENT $SCS_MEA_FEED_PLANE_VALUE $SCS_MEA_FEED_FEEDAX_VALUE $SCS_MEA_FEED_FAST_MEASURE 328 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

327 Changes from cycle version SW4.4 and higher A.3 Complete overview of the changed cycle machine and cycle setting data A.3 Complete overview of the changed cycle machine and cycle setting data Table A-1 Complete overview of the changed cycle machine data - from cycle SW SW HF3 CYCLE SW CYCLE SW N51071 $MNS_ACCESS_ACTIVATE_CTRL_E N51072 $MNS_ACCESS_EDIT_CTRL_E N51073 $MNS_ACCESS_SET_SOFTKEY_ACCESS N51199 $MNS_ACCESS_WRITE_TM_GRIND N51606 $MNS_MEA_INPUT_PIECE_PROBE[0] N52740 $MCS_MEA_FUNCTION_MASK Bit 0 N51606 $MNS_MEA_INPUT_PIECE_PROBE[1] Not applicable N51607 $MNS_MEA_INPUT_TOOL_PROBE[0] N52740 $MCS_MEA_FUNCTION_MASK Bit 16 N51607 $MNS_MEA_INPUT_TOOL_PROBE[1] Not applicable N51609 $MNS_MEA_INPUT_TOOL_PROBE_SUB[0.. 5] Not applicable N51610 $MNS_MEA_TOOLCARR_ENABLE Not applicable N51612 $MNS_MEA_MONO_COR_POS_ACTIVE Not applicable, function always active N51614 $MNS_MEA_PROBE_LENGTH_RELATE N51740 $MCS_MEA_FUNCTION_MASK Bit 1 N51616 $MNS_MEA_CAL_MONITORING N51740 $MCS_MEA_FUNCTION_MASK Bit 0 N51755 $MNS_J_MEA_MEASURING_FEED N51774 $MNS_J_MEA_T_PROBE_TYPE[0.. 5] N51776 $MNS_J_MEA_T_PROBE_ALLOW_AX_DIR[0.. 5] N51778 $MNS_J_MEA_T_PROBE_DIAM_LENGTH[0.. 5] N51782 $MNS_J_MEA_T_PROBE_T_EDGE_DIST[0.. 5] N51787 $MNS_J_MEA_T_PROBE_MEASURE_FEED Not applicable N54633 $SNS_MEA_TP_TYPE[n] N54632 $SNS_MEA_TP_AX_DIR_AUTO_CAL[n] N54631 $SNS_MEA_TP_EDGE_DISK_SIZE[n] N54634 $SNS_MEA_TP_CAL_MEASURE_DEPTH[n] N54636 $SNS_MEA_TP_FEED[n] N52605 $MCS_MEA_TURN_CYC_SPECIAL_MODE N52740 $MCS_MEA_FUNCTION_MASK Bit 1 N52248 $MCS_REV_2_BORDER_TOOL_LENGTH N52290 $MCS_SIM_DISPLAY_CONFIG N52740 $MCS_MEA_FUNCTION_MASK N52751 $MCS_J_MEA_MAGN_GLAS_POS[0] N52751 $MCS_J_MEA_MAGN_GLAS_POS[1] Table A-2 Complete overview of the changed cycle setting data - from cycle SW SW HF3 CYCLE SW CYCLE SW N54611 $SNS_MEA_WP_FEED[0.. 11] N54636 $SNS_MEA_TP_FEED[0.. 5] N54651 $SNS_MEA_TPW_FEED[0.. 5] N54652 $SNS_MEA_INPUT_TOOL_PROBE_SUB[0.. 5] N54740 $SNS_MEA_FUNCTION_MASK N54760 $SNS_MEA_FUNCTION_MASK_PIECE Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 329

328 Changes from cycle version SW4.4 and higher A.3 Complete overview of the changed cycle machine and cycle setting data SW HF3 CYCLE SW CYCLE SW N54762 $SNS_MEA_FUNCTION_MASK_TOOL N54764 $SNS_MEA_FUNCTION_MASK_TURN N54798 $SNS_J_MEA_FUNCTION_MASK_PIECE N54780 $SNS_J_MEA_FUNCTION_MASK_PIECE N54799 $SNS_J_MEA_FUNCTION_MASK_TOOL N54782 $SNS_J_MEA_FUNCTION_MASK_TOOL N54655 $SNS_MEA_REPEAT_ACTIVE N54740 $SNS_MEA_FUNCTION_MASK Bit 0 N54656 $SNS_MEA_REPEAT_WITH_M0 N54740 $SNS_MEA_FUNCTION_MASK Bit 1 N54657 $SNS_MEA_TOL_ALARM_SET_M0 N54740 $SNS_MEA_FUNCTION_MASK Bit 2 N54659 $SNS_MEA_TOOL_MEASURE_RELATE Not applicable N54660 $SNS_MEA_PROBE_BALL_RAD_IN_TOA N54740 $SNS_MEA_FUNCTION_MASK Bit 3 N55600 $SCS_MEA_COLLISION_MONITORING N55740 $SCS_MEA_FUNCTION_MASK Bit 0 N55602 $SCS_MEA_COUPL_SPIND_COORD N55740 $SCS_MEA_FUNCTION_MASK Bit 1 N55604 $SCS_MEA_SPIND_MOVE_DIR N55740 $SCS_MEA_FUNCTION_MASK Bit 2 N55606 $SCS_MEA_NUM_OF_MEASURE N55740 $SCS_MEA_FUNCTION_MASK Bit 17 N55608 $SCS_MEA_RETRACTION_FEED N55740 $SCS_MEA_FUNCTION_MASK Bit 5 N55610 $SCS_MEA_FEED_TYP N55740 $SCS_MEA_FUNCTION_MASK Bit 4 N55628 $SCS_MEA_TP_FEED_MEASURE N55630 $SCS_MEA_FEED_MEASURE N55630 $SCS_MEA_FEED_RAPID_IN_PERCENT N55632 $SCS_MEA_FEED_RAPID_IN_PERCENT N55631 $SCS_MEA_FEED_PLANE_VALUE N55634 $SCS_MEA_FEED_PLANE_VALUE N55632 $SCS_MEA_FEED_FEEDAX_VALUE N55636 $SCS_MEA_FEED_FEEDAX_VALUE N55633 $SCS_MEA_FEED_FAST_MEASURE N55638 $SCS_MEA_FEED_FAST_MEASURE N55642 $SCS_MEA_EDGE_SAVE_ANG N55761 $SCS_J_MEA_SET_NUM_OF_ATTEMPTS N55740 $SCS_MEA_FUNCTION_MASK Bit 17 N55762 $SCS_J_MEA_SET_RETRAC_MODE N55740 $SCS_MEA_FUNCTION_MASK Bit 5 N55763 $SCS_J_MEA_SET_FEED_MODE N55740 $SCS_MEA_FUNCTION_MASK Bit 4 N55770 $SCS_J_MEA_SET_COUPL_SP_COORD Not applicable, function always active N55771 $SCS_J_MEA_SET_CAL_MODE N55740 $SCS_MEA_FUNCTION_MASK Bit 15 N55772 $SCS_J_MEA_SET_PROBE_MONO Not applicable, function corresponds to tool type 330 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

329 Changes from cycle version SW4.4 and higher A.4 Comparing GUD parameters (regarding measuring functions) A.4 Comparing GUD parameters (regarding measuring functions) You can make specific basic settings per cycle machine, setting data (MD, SD). The following prefixes are defined: SNS_... Generally applicable setting data SCS_... Channel-specific setting data MNS_... Generally applicable machine data $MCS_... Channel-specific machine data The GUD parameters listed in the following table represent the contents of the GUD blocks GUD5, GUD6 and GUD7_MC up to version V7.5 where equivalent MD/SD is available as from version V2.7 / V4.4. The GUD are backwards compatible with existing measuring programs regarding their use. The GUD5, GUD6 and GUD7_MC modules are replaced by the PGUD (SGUD in the parameter display). GUD up to Version 7.5 _WP[x,0] _WP[x,1] _WP[x,2] _WP[x,3] _WP[x,4] _WP[x,5] _WP[x,6] _WP[x,7] _WP[x,8] _WP[x,9] _WP[x,10] From MD/SD version V2.7/V4.4 SD54600 $SNS_MEA_WP_BALL_DIAM[0...11] SD54601 $SNS_MEA_WP_TRIG_MINUS_DIR_AX1[0...11] SD54602 $SNS_MEA_WP_TRIG_PLUS_DIR_AX1[0...11] SD54603 $SNS_MEA_WP_TRIG_MINUS_DIR_AX2[0...11] SD54604 $SNS_MEA_WP_TRIG_PLUS_DIR_AX2[0...11] SD54605 $SNS_MEA_WP_TRIG_MINUS_DIR_AX3[0...11] SD54606 $SNS_MEA_WP_TRIG_PLUS_DIR_AX3[0...11] SD54607 $SNS_MEA_WP_POS_DEV_AX1[0...11] SD54608 $SNS_MEA_WP_POS_DEV_AX2[0...11] SD54609 $SNS_MEA_WP_STATUS_RT[0...11] SD54610 $SNS_MEA_WP_STATUS_GEN[0...11] _KB[x,0] _KB[x,1] _KB[x,2] _KB[x,3] _KB[x,4] _KB[x,5] _KB[x,6] SD54621 $SNS_MEA_CAL_EDGE_PLUS_DIR_AX2[0...2] SD54622 $SNS_MEA_CAL_EDGE_MINUS_DIR_AX2[0...2] SD54615 $SNS_MEA_CAL_EDGE_BASE_AX1[0...2] SD54617 $SNS_MEA_CAL_EDGE_PLUS_DIR_AX1[0...2] SD54618 $SNS_MEA_CAL_EDGE_MINUS_DIR_AX1[0...2] SD54620 $SNS_MEA_CAL_EDGE_UPPER_AX2[0...2] SD54619 $SNS_MEA_CAL_EDGE_BASE_AX2[0...2] _TP[x,0] _TP[x,1] _TP[x,2] _TP[x,3] _TP[x,4] _TP[x,5] SD54625 $SNS_MEA_TP_TRIG_MINUS_DIR_AX1[0...5] SD54626 $SNS_MEA_TP_TRIG_PLUS_DIR_AX1[0...5] SD54627 $SNS_MEA_TP_TRIG_MINUS_DIR_AX2[0...5] SD54628 $SNS_MEA_TP_TRIG_PLUS_DIR_AX2[0...5] SD54629 $SNS_MEA_TP_TRIG_MINUS_DIR_AX3[0...5] SD54630 $SNS_MEA_TP_TRIG_PLUS_DIR_AX3[0...5] Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 331

330 Changes from cycle version SW4.4 and higher A.4 Comparing GUD parameters (regarding measuring functions) GUD up to Version 7.5 _TP[x,6] and E_MESS_MT_DL[3] _TP[x,7] and E_MESS_MT_AX[3] _TP[x,8] and E_MESS_MT_TYP[3] _TP[x,9] and E_MESS_MT_DZ[3] From MD/SD version V2.7/V4.4 SD54631 $SNS_MEA_TP_EDGE_DISK_SIZE[0...5] SD54632 $SNS_MEA_TP_AX_DIR_AUTO_CAL[0...5] SD54633 $SNS_MEA_TP_TYPE[0...5] SD54634 $SNS_MEA_TP_CAL_MEASURE_DEPTH[0...5] _TPW[x,1] _TPW[x,2] _TPW[x,3] _TPW[x,4] _TPW[x,5] _TPW[x,6] _TPW[x,7] _TPW[x,8] _TWP[x,9] SD54641 $SNS_MEA_TPW_TRIG_PLUS_DIR_AX1[0...5] SD54642 $SNS_MEA_TPW_TRIG_MINUS_DIR_AX2[0...5] SD54643 $SNS_MEA_TPW_TRIG_PLUS_DIR_AX2[0...5] SD54644 $SNS_MEA_TPW_TRIG_MINUS_DIR_AX3[0...5] SD54645 $SNS_MEA_TPW_TRIG_PLUS_DIR_AX3[0...5] SD54646 $SNS_MEA_TPW_EDGE_DISK_SIZE[0...5] SD54647 $SNS_MEA_TPW_AX_DIR_AUTO_CAL[0...5] SD54648 $SNS_MEA_TPW_TYPE[0...5] SD54649 $SNS_MEA_TPW_CAL_MEASURE_DEPTH[0...5] _CM[0] SD54670 $SNS_MEA_CM_MAX_PERI_SPEED[0] 1) _CM[1] SD54671 $SNS_MEA_CM_MAX_REVOLUTIONS[0] 1) _CM[4] SD54672 $SNS_MEA_CM_MAX_FEEDRATE[0] 1) _CM[2] SD54673 $SNS_MEA_CM_MIN_FEEDRATE[0] 1) _CM[5] SD54674 $SNS_MEA_CM_SPIND_ROT_DIR[0] 1) _CM[6] SD54675 $SNS_MEA_CM_FEEDFACTOR_1[0] 1) _CM[7] SD54676 $SNS_MEA_CM_FEEDFACTOR_2[0] 1) _CM[3] SD54677 $SNS_MEA_CM_MEASURING_ACCURACY[0] 1) _CM[8] MD51618 $MNS_MEA_CM_ROT_AX_POS_TOL _CBIT[0] _CBIT[1] _CBIT[2] _CBIT[7] SD54740 $SNS_MEA_FUNCTION_MASK, bit 0 (measure workpiece) SD54740 $SNS_MEA_FUNCTION_MASK, bit 16 (measure tool) SD54740 $SNS_MEA_FUNCTION_MASK bit 1 (measure workpiece) SD54740 $SNS_MEA_FUNCTION_MASK, bit 17 (measure tool) SD54740 $SNS_MEA_FUNCTION_MASK bit 2 (measure workpiece) SD54740 $SNS_MEA_FUNCTION_MASK bit 18 (measure tool) MD51740 $MNS_MEA_FUNCTION_MASK bit 2 (measure workpiece) MD51740 $MNS_MEA_FUNCTION_MASK, bit 16 (measure tool) _CBIT[8] MD51740 $MNS_MEA_FUNCTION_MASK, bit 3 _CBIT[14] MD51740 $MNS_MEA_FUNCTION_MASK bit 1 _CBIT[15] SD54740 $SNS_MEA_FUNCTION_MASK, bit 3 _CBIT[16] MD51740 $MNS_MEA_FUNCTION_MASK bit 0 _CHBIT[0] MD52740 $MCS_MEA_FUNCTION_MASK bit 0 _CHBIT[1] MD52740 $MCS_MEA_FUNCTION_MASK bit Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

331 Changes from cycle version SW4.4 and higher A.4 Comparing GUD parameters (regarding measuring functions) GUD up to Version 7.5 _CHBIT[2] _CHBIT[10] From MD/SD version V2.7/V4.4 SD55740 $SCS_MEA_FUNCTION_MASK bit 0 (measure workplace) SD55740 $SCS_MEA_FUNCTION_MASK bit 16 (measure tool) SD55613 $SCS_MEA_RESULT_DISPLAY _CHBIT[13] SD55740 $SCS_MEA_FUNCTION_MASK bit 1 _CHBIT[14] SD55740 $SCS_MEA_FUNCTION_MASK bit 2 _CHBIT[15] _CHBIT[16] _CHBIT[17] SD55740 $SCS_MEA_FUNCTION_MASK bit 3 (measure workplace) SD55740 $SCS_MEA_FUNCTION_MASK bit 17 (measure tool) SD55740 $SCS_MEA_FUNCTION_MASK bit 5 (measure workplace) SD55740 $SCS_MEA_FUNCTION_MASK bit 19 (measure tool) SD55740 $SCS_MEA_FUNCTION_MASK bit 4 (measure workplace) SD55740 $SCS_MEA_FUNCTION_MASK bit 18 (measure tool) _CHBIT[19] MD52740 $MCS_MEA_FUNCTION_MASK bit 1 _CHBIT[22] SD54740 $SNS_MEA_FUNCTION_MASK, bit 19 _EVMVNUM[0] _EVMVNUM[1] _EV[20] _MV[20] SD55622 $SCS_MEA_EMPIRIC_VALUE SD55624 $SCS_MEA_AVERAGE_VALUE SD55623 $SCS_MEA_EMPIRIC_VALUE[0...19] SD55625 $SCS_MEA_AVERAGE_VALUE[0...19] _SPEED[0] _SPEED[1] _SPEED[2] _SPEED[3] SD55632 $SCS_MEA_FEED_RAPID_IN_PERCENT SD55634 $SCS_MEA_FEED_PLANE_VALUE SD55636 $SCS_MEA_FEED_FEEDAX_VALUE SD55638 $SCS_MEA_FEED_FAST_MEASURE _TP_CF _MT_COMP SD54690 $SNS_MEA_T_PROBE_MANUFACTURER SD54691 $SNS_MEA_T_PROBE_OFFSET _MT_EC_R[1.5] _MT_EC_R[2.5] _MT_EC_R[3.5] _MT_EC_R[4.5] _MT_EC_R[5.5] _MT_EC_R[6.5] SD54695 $SNS_MEA_RESULT_OFFSET_TAB_RAD1[0...4] SD54696 $SNS_MEA_RESULT_OFFSET_TAB_RAD2[0...4] SD54697 $SNS_MEA_RESULT_OFFSET_TAB_RAD3[0...4] SD54698 $SNS_MEA_RESULT_OFFSET_TAB_RAD4[0...4] SD54699 $SNS_MEA_RESULT_OFFSET_TAB_RAD5[0...4] SD54700 $SNS_MEA_RESULT_OFFSET_TAB_RAD6[0...4] _MT_EC_L[1.5] _MT_EC_L[2.5] _MT_EC_L[3.5] _MT_EC_L[4.5] _MT_EC_L[5.5] _MT_EC_L[6.5] SD54705 $SNS_MEA_RESULT_OFFSET_TAB_LEN1[0...4] SD54706 $SNS_MEA_RESULT_OFFSET_TAB_LEN2[0...4] SD54707 $SNS_MEA_RESULT_OFFSET_TAB_LEN3[0...4] SD54708 $SNS_MEA_RESULT_OFFSET_TAB_LEN4[0...4] SD54709 $SNS_MEA_RESULT_OFFSET_TAB_LEN5[0...4] SD54710 $SNS_MEA_RESULT_OFFSET_TAB_LEN6[0...4] E_MESS_D E_MESS_D_M E_MESS_D_L MD51750 $MNS_J_MEA_M_DIST MD51751 $MNS_J_MEA_M_DIST_MANUELL MD51752 $MNS_J_MEA_M_DIST_TOOL_LENGTH Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 333

332 Changes from cycle version SW4.4 and higher A.4 Comparing GUD parameters (regarding measuring functions) GUD up to Version 7.5 E_MESS_D_R E_MESS_FM E_MESS_F E_MESS_FZ E_MESS_CAL_D[2] E_MESS_CAL_L[0] E_MESS_MT_DR[3] E_MESS_MT_DIR[3] From MD/SD version V2.7/V4.4 MD51753 $MNS_J_MEA_M_DIST_TOOL_RADIUS SD55630 $SCS_MEA_FEED_MEASURE MD51757 $MNS_J_MEA_COLL_MONIT_FEED MD51758 $MNS_J_MEA_COLL_MONIT_POS_FEED MD51770 $MNS_J_MEA_CAL_RING_DIAM[0...11] MD51772 $MNS_J_MEA_CAL_HEIGHT_FEEDAX[0...11] MD51780 $MNS_J_MEA_T_PROBE_DIAM_RAD[0...5] MD51784 $MNS_J_MEA_T_PROBE_APPR_AX_DIR[0...5] E_MESS_SETT[0] SD55740 $SCS_MEA_FUNCTION_MASK bit 14 E_MESS_SETT[1] SD55740 $SCS_MEA_FUNCTION_MASK bit 15 1) For parameters SD54670 to 54677, there are two data sets, indices 0 and 1. Note: Data set with index 1 should always be used for GIV 2.7/4.4. Data set with index 0 should always be used from GIV 4.5 and higher. GUD up to cycle SW _RF From cycle SW N55640 $SCS_MEA_FEED_CIRCLE 334 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

333 Changes from cycle version SW4.4 and higher A.5 Changes to names of cycle programs and GUD modules A.5 Changes to names of cycle programs and GUD modules The following measuring programs have been renamed or deleted from measuring cycle version 2.6: Cycle Name of GUD up to Version 7.5 Cycle Name as of Version 2.6 CYC_JMC CYC_JMA Cycle198 Cycle199 Cycle100 Cycle101 Cycle105 Cycle106 Cycle107 Cycle108 Cycle113 Cycle118 Cycle972 E_SP_NPV CYC_JM GUD5 GUD6 GUD7 GUD7_MC Cycle131 Cycle132 CUST_MEACYC CUST_MEACYC Program is no longer available. Program is no longer available. Program is no longer available. Program is no longer available. Program is no longer available. Program is no longer available. Program is no longer available. Program is no longer available. Program is no longer available. Program is no longer available. Program is no longer available. Module no longer available. Module no longer available. Module no longer available. Module no longer available. Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 335

334 Changes from cycle version SW4.4 and higher A.5 Changes to names of cycle programs and GUD modules 336 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3

335 Appendix B B.1 Abbreviations Abbreviation CNC DIN I/O GUD JOG MD MCS NC NCK NCU WO PLC SL Software WCS Meaning Computerized Numerical Control Computerized numerical control Deutsche Industrie Norm (German Industry Standard) Input/Output Global User Data Global user data JOGging: Setup mode Machine data Machine coordinate system Numerical Control: Numerical Control Numerical Control Kernel: NC kernel with block preparation, traversing range, etc. Numerical Control Unit: NCK hardware unit Zero point offset Programmable Logic Control Controller Cutting edge position Software Workpiece coordinate system Programming Manual, 10/2015, 6FC5398-4BP40-5BA3 337

336 B.2 Documentation overview Appendix B.2 Documentation overview 338 Programming Manual, 10/2015, 6FC5398-4BP40-5BA3